Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: Leeway on January 23, 2011, 04:04:44 PM
-
Trying to finally setup my lathe using Turn instead of mill.
I normally use 3 tools on the lathe. A parting tool that I also turn my profile with. It is on a QCTP. I set machine 0 with this.
Then I use a spot drill.
Next is a drill bit.
Question is when I have setup all my tool tables with the correct offsets, do I then need to use the same offsets on tools in my Cam software?
Dolphin Turn.
It seems a little redundant to me.
Also, what would be the file name for my XML in Mach 3 Turn?
I looked, but it wasn't really apparent to me.
Thanks in advance.
-
Yes, the numbers in the tool table are actually the offsets, so for example T0101 would be tool 1 offset 1, you can have any offset you wish (up to 99) called with a tool number, but obviously it needs to correspond to what you have set in the table for that tool.
What I mean by that may be better explained by my screenshot, that shows the tool numbers with their associated offsets, this is because I have two turrets on my lathe with 6 positions in each turret. The front turret has quick change holders so I have a lot of tools set up in holders ready to place there and thus I have many offsets for these tool positions.
In Dolphin the offset number will default to the same as the tool number so if you have the offsets and tool numbers the same then there is no need to do anything but if they are different like a lot of mine are then you need to enter the offset value in when you load a tool, its done Via the X offset value, I have attached a screenshot showing the tool number and offset and the code as it comes out, its T0921 my internal threading tool.
The xml will have the name of the profile you are using, if its the standard lathe one it will be Mach3Turn.xml, if its a custom one then it will have the name of what you called it.
Hood
-
Great info and a big help especially with the screen shots. Thanks a bunch for this. I have another question.
What post processor are you using in Dolphin?
Thanks again.
-
I am using one I made up to suit my twin turret setup. I basically took the Mach one and altered it quite a bit, this is the changes I made.
:T2 = {
Changes include:
Toolchange position is for turret in use and not turret that is next.
Threading changed to G76 rather than G32
Coolant is dependant on tool used
M5 will be issued befor M3/M4 if spindle is to be reversed
Modality has been changed so that code is only written if position will change
Arcs are reversed if front turret is in use
X values negated if front turret in use
Drill cycles now produced long hand rather than canned cycles
G90.1 inserted in preamble
}
:T3 = {
Changed threading Rules for both External and Internal to produce correct thread
height from nominal and pitch dimensions. For external it is the nominal value for
the thread that is used for start and end points. eg M12 is 12mm and for Internal it is the nominal minus
the pitch, eg M12 would be 12 - 1.75 = 10.25
Hood
-
Thanks again.
Things are looking up here now.
It threw an error in the code because I was using diameter post in radius mode.
At least I think so.
Changing it fixed it.
One more simple question.
I have it setup now so that when I jog with the up key from 0, the x moves into -. The Z is like the arrow keys work with left being -.
Is that correct for a lathe?
I know some guys and machines code them a bit different.
-
You can have the keys which ever way you wish but my preference is up arrow is positive, then again I have the rear turret as the default turret so it makes sense for me. Having said that I never use the jog keys for jogging, I use the MPG for that.
If you need a hand with changing the post processor in any way I can try and help, not great at VB and such but will try.
Hood
-
Sounds good to me. Thanks.
I just have a gang tool setup. Kinda.
I do have a QCTP that I use and it is at the front of my X table. Behind it I have two positions for drilling or boring. I can also do that with the QCTP, but I like to have the three tools I need on there at once so no tool changes.
So far, it is all working on the computer.
I will hook it up to the lathe and try it out later.
Thanks again. Fingers crossed. ;)
-
There are a couple things that I have noticed about the post. It won't set the zero before a tool number when it is a single digit tool number.
That isn't a problem any longer. I just redid my tools and offset to start with 11 and go from there.
It also does some reference move and I have no idea why it puts that in there. It moves X back 1.96 and change. Something with a G28. Not a problem though. It's going the right way when it does it.
Other than that, the posts are coming out good when I tell the DT what it needs. I struggled with DT for some time previously and just left t alone a few times.
After looking through documentation for Lazy Turn, Dolphin became simpler to operate as well.
I have to blame Microsoft too though on some of it.
I have to run DT in XP mode. Another work around, but hey, once you know it it's all good. Thanks again for the help.
-
Not sure what you mean about the zero before the tool number, the PP I have does, maybe you are using the Mach2 one as I think tool numbers were called in a mill type fasion in it. With mine if I call tool3 offset 3 it will produce T0303.
Dont get any G28's in mine either, I have attached the standard Mach3 PP that I had, see if thats the same.
Hood
-
I figured out the offset move. I misspoke on the axis. It is Z that moves to safe Z that I set in DT. That is actually good, since my drills that are offset just a bit past the cutter 0, so the safe travel is what I was looking for.
I am attaching an amended code that I modified. Mods are in ().
Every one of my bushings will use this exact drilling routine, so that part I can cut and paste. It is only the profiles that will change.
Today I cannot get Mach3turn to even post any tool numbers.
It did so last night, but not today. That is weird.
I am using the latest version of Mach 3. Version R3.043.022
I am using Mach blue turn for the screen, but that shouldn't matter.
I can try the latest lock down version if you think it might help.
I also noticed that Mach 3 screen doesn't handle offsets very well. ;) This little bushing shows up looking much like a wagon wheel mounted on an axle. Not a problem though. Just a mention.
Thanks for wanting to help with this.
-
That is either a mill post processor or an old Mach2 one you are using as the tools in Turn should be of the format Taabb where aa is the tool number and bb is the offset number. Yours is calling Taa and the offset coming in the form of Hbb which is the way mills do things and I think Mach2 Turn maybe also did it.
Heres a screenshot of what I see.
Hood
-
I was actually using the same post, but for radius mode with an R in place of the D.
I did use your post and changed it to Diameter mode in DT, but now I get a PP error.
"G83" at line 1 in Rule NPECK
syntax error
DT shows me that and then want me to change the post.
It outputs very little because of this.
Thanks.
-
Ok just downloaded and changed the radius post so that it spits out the correct format for tools, see if this works.
Hood
-
I did use this post, but it made no change.
I even tried an older version of Mach 3 and it still will not post a tool number in the Mach 3 screen.
I will try the original screen again, but I don't think that is the issue.
No change on the Original screen.
If it isn't setting the tool number, then it can't set the offsets either, correct?
DT knows the offsets though.
Do I even need them in Mach 3?
-
You sure you chose the correct post? Just that with your previous code the tools were as you would expect for a mill and that one I posted should have the tool numbers in the correct format, ie T0101
Heres a screenshot of the fist part of code I have just produced with it.
Hood
-
You did it right.
It was my fault.
The last file when I changed the post, it also changed the file type tp PUN and I didn't realize that. Now that I uploaded the new file from the correct post with the correct extension, it works. Devil is in the details. ;)
Thanks.
-
Ha ha yes been caught out that way myself a few times.
Hood
-
Hmm.
Now that post is throwing all my offsets out double. As if it's a post for Diameter.
I have confirmed that both M3T and DT are set to radius mode.
As soon as the code initiates even though it doesn't show an axis move, it sets the DRO's to a positive value of my offsets. At that time program extents are shown double as well.
Did you modify a radius post or diameter post? It could very well be me too, but I haven't seen this action before.
-
Never mind on that question. I see it is a radius post. Says so at the top.
-
Its the radius one downloaded from Dolphin USA and just changed the tool number/offset.
Hood
-
I've got it cutting my parts finally, but still see some issues. I'm pretty sure I can attribute them to me. ;)
When I setup my tools in Dolphin Turn, then set them up in Mach 3 Turn, it sets the offsets twice. That gives me double offsets. Mach doesn't travel to the expected offset. It just posts it in the dro after the initial tool change move. I delete the offsets in Mach and everything works correctly. It has to be something that I don't have my head wrapped around yet. I do, however, get my tool numbers showing up. Without the offsets in Mach though, the tool numbers are not important.
Any thoughts on that?
Thanks.
-
Not really sure what you are meaning unless you are asking actually setting offsets in Dolphin. Can you attach the cnc file and also your Mach tooltable.
Hood
-
It would not let me upload the files here. I did put them on my website too, but can't see them in a browser.
They aren't real big if you want me to email them. One is 19 KB and the other is 7 KB.
Thanks.
Lee
-
Just zip and attach and the forum will accept.
Hood
-
Duh! My mind is fried. :o
-
Ahhhhhhhh cant test here, dongle is at home, will check it out later tonight.
Hood
-
I am not really seeing where your problem is, it seems fine here, then again I dont use the standard lathe screen so unsure what all that home world stuff is.
Can you attach the code you get.
Hood
-
Here it is.
Unchanged. I do have to dress it up some, to actually use it though.
-
Ok as said I dont use the standard screen so cant tell you what buttons you want to press but I would think the method should be the same. Well not the same as I do as I have accurate homing and have a home off value for my master tool.
Anyway what you need to do is make sure tool 1 is loaded and then move it to the dia and set the X DRO to the dia, then do the same for the Z, zero it when its at the end of the stock.
Hood
-
Do you mean my master tools offset on X should be set at like 9/16"? Zeroing the dro this way really throws everything out of whack for me. If I use tool offsets in M3T and in DT, they don't offset each other, but double in the DRO. To get to the tool then, it has to travel like 7.5". My X only has just over 5" of travel, so that ain't working.
I am using radius mode in both though.
I will try Diameter mode in both and see how that works out.
-
Sorry forgot you worked in Rad mode, have never seen the attraction to rad mode but some seem to prefer it, personally I think its much easier working in Dia.
Not understanding what you are meaning by setting the offsets in Dolphin, how are you doing that?
What normally you do is have Mach take care of offsets by having them in the tool table and the CAM basically produces code to cut at whatever radius/dia you tell it.
So what you do is have one tool as master and zero the Z on the end of the stock or maybe set it positive by the amount you will be facing off. The tool is then placed against the OD or you can take a light cut and measure the OD and you enter half that value into the X DRO (1/2 because you are in Rad mode) That is now your master tool set, no offsets in the table but work offsets. Next you change tool with the Taabb call and then move the tool to the same as before and then the difference from the master tool is entered into the tool table for the new tools X and Z, then next tool etc.
In the end your tool table has no offsets for master but offsets for the other so no matter which tool you call if you command it to move to Z0 it will go there, same for X values commanded.
Hood
-
Just had another look at your CNC file and it seems like it may be in Dia mode in Dolphin, could that be your problem? I am not 100% sure if it is definitely Dia mode though as it may just be my setup here that changes it to Dia mode as that is what I have Dolphin set as default for and maybe its changed your file when I opened it.
Hood
-
I did have both in radius. Tried Diameter too without a lot of success. Here is a screen shot of the tool offsets in DT.
-
Ah Ok thats your problem then, dont enter any offsets there as you want Mach to handle the offsets in the tool table.
Hood
-
Hi All,
I have been following this thread for a few day now. I gave up using Tool Tables for Gang Tooling in CNC lathes controlled by Mach3. I now use G52 Offsets for all tools in the Gang setup.
Here is my experience and solution to the problem.
http://www.cjh.com.au/Gang%20Tool%20Block%20Offsets%20for%20CNC%20Lathes%20under%20Mach3%20Control.pdf
Regards
Chrisjh
-
Chris,
I use the tool tables in Mach for my lathe which has a front and rear turret and dont have any issues at all. There is one thing you have to make sure of and that is you have ALL tools set up as either Front or Rear in the Tooltable. Having a mixture of both is a disaster and will lead to all sorts of problems. Because my default turret is the rear I have mine all set as rear, even the ones on the front turret. That means the X axis moves positive when its moving away from the operator so any tools I have on the front turret need to be programmed with negative X values and also when entering values in the tool table you need to remember to enter the negative diameters into the DROs before sending them to the tool table. I have attached a screenshot of the DROs for entering the values and the buttons that then enter these into the tooltable (first is my screen, second is standard but both are the same DROs and Buttons). So what I would do is for example if a tool is in the rear turret I move the tool to the dia of the stock and enter that into the X Val DRO and then press Set X button ( Part Zero X button on standard) and that will put the offsets in the tooltable. Now if I have a new tool and its on the front turret if I touch off the Dia it is past the zero point of my axis so its X values are now shown as negative. I again touch off the Dia as before but this time the value entered into the DRO would be a negative value.
It works extremely well for me with my quite complicated setup and I see no reason it would not work on a gang tooled lathe as long as you remember that in the tool table all tools need to be either Front or Rear but never a mixture. Your method obviously also works for you.
Hood
-
Thanks a bunch, Guys. I really like that tool setup. Looks like it works out great.
There is obviously more than one way to wrestle this mule. I have tried every different configuration possibility at this point between M3T and DT. I am spoiled about the dro's showing me the exact values of where the tools are in relation to the spindle. I guess that is because I hand coded these before, so it is a simple matter to get my mind around that concept.
The two programs were competing against each other and cancelling or doubling offset values depending on how it was setup. Of the two modes, radius seems to allow the dro's to follow exactly along with offsets when they are programmed in DT. This doesn't happen in M3T. What happens there is it goes into machine coordinates. It just posts the opposite of your offset and then travels to 0 in the dro, which is your offset. This makes it more difficult for me to dress up the gcode as output by DT.
It does need some dressing too. It overtravels back to home too often. It doesn't allow single axis moves with each type of operation. It does for some, but not all.
Sooo.....the best for me is not tool offsets in Mach. Load them in DT instead. Keeps dro's in the actual program coordinates. That is a single system and easy to keep track of and recognize what it's doing at any given time.
These are production parts, so these offsets won't really change.
I'll always just reset them there.
I'll snap a few pictures of the gang setup now.
It is similar to what I had before, but now the drills are on one plate and have collets for changing drills.
I do use boring bars sometimes, but they go in the QCTP instead of a collet.
That is the best thing about Mach3. There are so many ways to do something with it that you are bound to find one that works for what you want to do.
-
Hi Hood,
I took your experienced advice ages ago and setup using one tool post only. In my case, I selected the front tool post option, so tools that cut from the rear side have negative values of X whilst tools that cut on the operator side operate in positive values of X.
Using the Tool Table and calling individual tools works fine with Mach3. However it was not suitable for my gang setup (and I suspect most gang tool setups). The problem I had in the gang setup was, when a tool whose centreline was located, say, 100mm from the Master Tool position was selected, the cross slide would try to travel to a position beyond the X+ limits before returning to the correct position.
I proved that Mach 3 Tool Table calls worked OK with a tool whose centreline displacement from the Master Tool was 40mm. When this tool was called from the Tool Table, the initial travel from the Master Tool Position was towards the operator (positive X direction), then return to the correct position 40mm (in a negative X direction away from the operator) from the Master Tool position. The first movement stopped just short of the X+ Limit Switch. Any other tools greater than 40mm from the Master Tool simply tripped the limit switch on the first, unnecessary excursion.
I suspect that double movement I was witnessing has something to do with the maths algorithm within Mach3. Because I couldn’t do anything about the algorithm, I had to seek an alternative solution.
The total Cross Slide travel between limit switches in my setup is approximately175mm so I have work within these limits.
You are correct in that there are many ways to skin a cat. This Mach3 journey, for me, has been long and rewarding. Still learning and trying pass on my experience in this fascinating hobby.
Leeway,
It was one of your YouTube videos that got me started down the gang tool setup path. I thank you for these videos. Love the Pink Panther!! (Still in my favourites).
Here is one for you. http://www.youtube.com/watch?v=gsw5JtYMGSI&feature=mfu_in_order&list=UL
Regards
Chrisjh
-
However it was not suitable for my gang setup (and I suspect most gang tool setups). The problem I had in the gang setup was, when a tool whose centreline was located, say, 100mm from the Master Tool position was selected, the cross slide would try to travel to a position beyond the X+ limits before returning to the correct position.
Regards
Chrisjh
I do not understand this bit at all, you are saying when you called a tool it would go off before coming back? If so then were you using a toolchange position from within the m6 macro?
I can call any tool I like and the axis will never move unless commanded, the DROs will change to show the position of the tool but no motion at all until I command a move.
Hood
-
Hi Hood,
Attached is a diagram showing examples of how the tools move from one position to the next when called from the Tool Table.
The other drawback is that CSS was also affected because Mach3 thinks that the new Position of the tool is at a much larger diameter, so the spindle rotates at minimum speed. That is, it appears to behave like the job is larger in diameter by a factor of the tool offset distance.
Its been quite a while since I witnessed all this so my recollection is sketchy. I think I recall seeing the X DRO indicating the larger diameter. I suspect that this is because Mach3 thinks that the job is bigger in diameter that it really is when a tool with an X position greater than the Master Tool.
Regards
Chrisjh
-
Hi all I had this kind of problem with gang tooling. what worked for me was a different fixture offset for each tool position. + tool offsets for each tool
Worked good for me.
Roy :)
-
Ahh. Fixtures. That is something that I haven't toyed with. That may actually solve the dro jumping to a negative of the tool offset and then traveling back to zero to cut at the offset. That is the only thing I didn't like about it. I couldn't watch the DRO's and adjust my code accordingly.
I can't get Dolphin to produce code that I can use.
It must be tuned up by hand.
Since all my tools are on a gang setup, there is no need for basic parts to have a tool change.
I ignore tool change in M3T for these parts. DT puts a spindle stop M5 in at each tool.
Then at each tool, it goes to safe Z and then back to zero using a G28. No idea how that gets in there. ;)
Since all three tools are not at zero in Z, they cannot travel in X at zero to the offsets. They have to do traveling at Z1. I need single axis moves instead of both.
I am wondering if Exact Stop might help there?
Something Odd that M3T is doing too with G83.
The first deep drill cycle I use works great.
After the first part is parted, the second deep drill cycle is doing stuff it shouldn't. Like initially plunging to new cut depth at full rapid. That's okay, but then it will G01 back to zero, then rapid back a few times until if finally starts to do the deep drill cycle like it should. I'll try to get a video of it.
I did find the zip file on here concerning this and did install the files in the correct folder, but not getting different results yet.
I still have a lot to learn about both M3T and DT, but I am producing parts again. :)
-
Yes, hated that spindle start stop crap in Dolphin as well, so I removed it :) Now the spindle will only stop if it is to reverse or at the end of the code :)
In Dolphin you can have a Go To move and as you can see in the attach pic you can specify if you want one axis to move first, can have incremental moves etc etc.
G83 doesnt work for me in Turn, thats why I set Dolphin up to do it long hand rather than canned.
Still not sure why you guys with Gang tools have problems with the Tooltables but as long as you find a way to work that suits yourself thats all that matters.
Hood
-
I just started using that goto thing. It works great, but it doesn't remove unwanted moves. It still does those. Not a big deal to edit the code though for this dozen or so bushings it does mainly. It only takes maybe a minute or two to set them right.
My issue has been that my drills are in the negative Z. Just a hair, but still in the -.0147" and -.0324". This means you cannot move to the X offsets until you are at like Z.0325". I use Z1.0"
It always has the X moves first in Dolphin, so a little mod here and there and viola.
I guess I will resort to doing the deep drills long hand as well.
Once done, thats it.
Then I will turn some darn profiles. Like chess pieces and things. That was my reasoning behind doing this stuff now anyway. ;)
If feels pretty good to have tackled it and set it up to be able to do cad drawing in a proper turning format.
I shot a video earlier, but it looked bad and sounded worse. I was way too close to the action. ;)
I'll do another and get it posted up soon.
Thanks.
-
You would I imagine be able to alter the post processor so that it doesnt do a X move when it goes to the toolchange position. I have already changed mine so that it looks to see which turret is being used and it will go to that turrets toolchange position, previously it was goin to the toolchange position of the next tool. If that was the other turret then it would be a disaster as tools would smash into the work.
Hood
-
Try this PP. I have altered it so that hopefully it will ignore any values set in the X toolchange box and just go to Z Toolchange position when you call a new tool.
I am unable to test it as my dongle is at the workshop so make sure you look thoroughly at the code before you try and run it.
BTW I presume you are setting a toolchange position like in the pic? Well not like in the pic but I am meaning you are entering a value for the toolchange position arent you?
Hood
-
Oh I forgot to remove the M5 from the toolchange section, if the above is working and you want the spindle to keep going when changing a tool then let me know and I will alter it.
Hood
-
Tried that one and it had about 25 post processor errors. Tried it twice.
Here is where I set tool change.
-
Ok probably have a syntax error, will have a quick look biut if I cant find it I will have to wait until I have my dongle here so I can see where its going wrong.
BTW you can also set the toolchange position amongst others by clicking on the lathe pic at the right, well thast if you have the screen set up that way.
Hood
-
Ok try this.
Hood
-
Actually this might be better, this is my last attempt before I have the dongle so if it doesnt work it will be tomorrow night before I can try again.
Hood
-
Just tested it here and it seems to be doing what its meant to, previous ones I had commented out some lines but used the Mach way of commenting and forgot the PP uses a different method.
Anyway see if it works like it should and if not let me know whats wrong. BTW I have it set for Turret 2 toolchange position which I think is the default for front turret in Dolphin, if its the opposite way on yours let me know and I will change that, only take a few secnds for that :)
Hood
-
Thanks a bunch.
That one works much better.
The one with all the errors still spit out the code and it didn't look bad.
The drilling routines are much smoother now without the G83 as well.
I ordered a new camera. I have had this one for nearly 8 years now. Needed an update. Just bought a little Kodak for less than $50. Supposed to have hi def video and 12.3 MP.
I'll shoot some video with that when it comes in.
The old one is a Vivitar. The shutter covers flopped around all the time and a few other things were starting to fail as well.
Video never did work right. Only started recording sound a few years back.
It was time. ;)
-
Ok thats good, is there anything else thats not working correctly as I might manage to change it. Not great at stuff like this but did manage to get mine working a lot better for the twin turret lathe I have.
Hood
-
I intend to goof around with the fixture tables just to wrap my head around them.
I'll let you know, but right now, it spits out pretty good code.
If my drills were set in the positive, I would not have to adjust the code at all.
I ban slice off a bit if I wanted. I think I may do that anyway.
As it stands, the way I have it setup, there are no negative X moves. Everything is done in the + side. Parting stops at zero, but everything is bored through, so doesn't really need to cut that close.
Working great now.
I am going top give my brain a break though. Who said the old dog new trick thing was true? It ain't. Not that old, but ain't no spring chicken either. :)
Thanks again for all the fantastic help from every. Especially Hood.
I will still post a video link in this thread when I get it done. I like to see threads that work out in the end. Makes them well worth the read and effort involved to document the issues.
-
Look forward to the vid :)
Hood
-
I still have some fine tuning to do to the code to get it to rapid in on the drilling. I got carried away with the zoom on this camera as well.
My other would not zoom in video mode.
http://www.youtube.com/watch?v=6nNCWBqJOPU
-
Looks like its working well, bit of vibration due to amount sticking out the chuck on the first part but looks like the surface finish is fine so no probs :)
Regards the pecking, your PP is set up I think to have it as a canned cycle, that is broken in Turn so wont rapid back in, I altered my PP to make Dolphin calc in long hand rather than canned, load this and see if its better for you, the options in Dolphin should now work for drilling cycles and the code should be long hand rather than canned.
Hood
-
Thanks for that. When you said long hand previously, I did it really long hand. ;)
The first video I showed is as the drill code is produced from DT.
I will attach a screenshot of how I set that up to cut in DT.
Then in the code it produced, I modified it for this second video.
After a drill cycle and a retract, I would copy and paste that depth on the next line with a G00 instead of G01. Then from there it would feedrate drill the next step. Pretty quick to actually do. Makes the cycle a lot cleaner and faster.
That is finished code for my production parts.
Here is the link to video 2.
http://www.youtube.com/watch?v=I2nH1NWm4dg
Next up will be some actual profile turnings probably in aluminum. Brass ain't cheap. :)
I also trued up my chuck before that video and reset my motor drive acc. It is a little smoother. This lathe is actually pretty light and not bolted down yet. I knew I had to move it soon.
The chuck in the first video was out by .003". Thats a good bit and think it happened during the few crashes it encountered. :(
It is now set at .0005". I can live with that.
-
Okay!
I think I have seen the error of my ways. ;)
Setting the offsets in DT was fine while they remained constant. However, tools wear. Setups change just a hair even with temperatures. I noted that before and thought it wouldn't change that drastically, right.
Well I loaded up the mill screen to fine tune my steps per inch. I only bettered them by a fraction, but it was enough to throw off my prefectly set offsets. :(
No problem if you are doing them in M3T and using the tool tables. Then you just set each by touching and that adjusts the tools offsets for you. Then you could use the same code, providing you didn't let Dolphin Turn handle them all. ;)
Okay then. All a wash at this point.
Redoing it all now to see how it all works out.
I'll holler.
-
Well, after some testing, I gotta say it works great using the tool offsets in M3T.
I removed all the offsets from Dolphin turn. The code stays the same now. Oh yeah, the last PP you posted works well. It still doesn't rapid back into the previously bored depth, but as I mentioned, it's an easy copy/paste fix.
While I can no longer follow the code on screen like I could before to see what it's doing, M3T is smart enough to deal with it like it should.
Now when I change up anything, all I do is update the tool chart and touch off each tool and viola.
Not sure why I was so confused to start with, but there you have it.
It works great.
I will post another link to a different video when I get a chance to run some profiles.
Thanks again.
-
I also set all my tools at 0 on Z depth. Those collets I added makes that a simple task. Nothing crashes now. ;)
-
I couldnt understand either why Gang tooling would not work with the tool table offsets but good you got it working as its really simple to set up and keep track of.
Regards the peck in the last PP, it should rapid back in, can you attach your .cnc again so I can figure out where its going wrong for you.
Hood
-
Here you go.
-
Seems to be working fine here, changed the Z transition to 0.05" and it rapids back to 0.05" before the last depth then continues, see code
; TOOL definition
N180 G0 Z1.0
N190 ( Twist Drill / Center Drill )
N200 M06 T0303
N210 G94
N220 G97 S3600
N230 X0.0 Z0.05 G94
N240 G01 X0.0 Z-0.1607 F8.0
N250 G00 X0.0 Z0.05
N260 X0.0 Z-0.1107
N270 G01 X0.0 Z-0.3213
N280 G00 X0.0 Z0.05
N290 X0.0 Z-0.2713
N300 G01 X0.0 Z-0.482
N310 G00 X0.0 Z0.05
N320 X0.0 Z-0.432
N330 G01 X0.0 Z-0.6426
N340 G00 X0.0 Z0.05
N350 X0.0 Z-0.5926
N360 G01 X0.0 Z-0.8033
N370 G00 X0.0 Z0.05
Have attached the .cnc so you can see the settings.
If its not right let me know and I will see if I can figure it out.
Hood
-
I see what you mean. Yes it does work like this. I wasn't trying the deep drill. I was doing the long long long hand. ;)
Now then the only other thing I was adding was goto at the end of the program. I send it back to zero all.
Thanks a million for this PP. I'm sure it may work well for others too.
One other thing I will mention.
When I have Mach set to stop at tool change, upon clicking cycle start, it posts an error that says no spindle speed posted yet.
I use ignore tool change mostly. I just test code one tool at a time first initially. A little safer that way.
I have moved the S2400 up one line to solve this.
Not sure why it sees that as a problem, but doesn't when ignore tool change is used.
-
I think probably it is best for you to choose auto tool changer however I think I know what the problem is as I to had that problem with the first Mach3 post I used from Dolphin, give me a few and I will change things and see if it helps you.
Hood
OK try this
-
Now you have gone and made it perfect. ;)
Thanks a bunch for all the help. I did take your advice and use the auto tool change method.
No more complaints.
-
No probs, its quite easy to make these types of changes in the post processor :)
Hood
-
I did change mine that I use for Sheetcam some, but it is also easy to screw one up.
-
Yes but secret is when you make a change dont save it, use save as instead, that way if you screw up you still have the original. I have about 30 different ones for my lathe LOL, it took quite a while to get it working with front and rear turrets and even yet its not perfect as for a boring bar on the front turret I need to tell the cam its on the rear and for a front turret turning tool for some strange reason the Cam needs to be told its aproaching from the rear.
I have given up messing with things for the moment as I am sure this has a bit to do with the way Mach handles front/rear tools and Brian is reworking things so maybe in about 20 or 30 years time we will have a new updated Mach3Turn to play with ;D
Hood
-
That is also why I keep several older versions of Mach on file in my backup drive.
I could tell just by the way that you named the files, that you have had experience doing so. :)
-
Yep, my latest one is called
AlmostFingThereButItWillHave2Do.ppr ;D
Hood
-
I am setting Mach3turn for the fist time on my mini lathe. I can use one tool fine, but when I set the offsets with the tool table page, the only offset registering is the last one I do. Can someone advise me. I would like to set all my tools from machine zero. Do I have to enter in the offsets manually on the offset page. Mach3mill is so much easier with Z offsets and multiple tooling everything is set from Z machine zero for your reference heights. and you leave X and Y alone so you can program G54 and up. At work, my Fanuc controls on the lathes reference every tool from machine zero when you teach in X and Z.
Has anyone had success with Mach3turn and multiple tools. If so, how did you do it. Thanks for any help and advise.
Martyondrums ???
-
When you do your touch offs after the initial Zero tool, you must make sure that the tool you are now touching off is up and listed in the DRO.
Insure the proper tool number is there and do the touch off thing and Mach will automatically load that offset for you in the tool table.
Be sure to save the tool table when you close Mach.
-
Heres a vid I did of one way to set up tools, I now have limits on the wee lathe so will have to do another showing the method I use with homes.
http://www.youtube.com/watch?v=mWnfioI3G0E
Hood
-
I believe that is what I was doing. I noticed that when I try to change tool numbers in the upper left DRO I sometimes had to click two or three times before it would except the number I was entering. And sometimes I had to exit out of the tool table page and go to manual page and then out and back into the tool table page before I could enter a number. All in all, after placing the diameter value and the Z value in the lower DRO's I would check the offset page by selecting edit and the offsets would still be zero. Could there be a glitch in my software copy? Maybe I should reisnstall it. What version is recommended?
Martyondrums
-
I think that may be a problem with the version you are using, is it 066 or 067? I had similar issues with these versions and Turn so went back to 057.
Brian was told but doesnt look like he bothering, probably would be different if it was issues with Mill.
Hood
-
I believe I am using 066. I will check tonight and download 057 today to reload it. I have mill on a differant computer so it won't interfere with the older version. I watched the video HoodScotland. Is this you? Anyway, maybe I an doing the touch offs wrong. I will try this method first to see if that is my problem. Thanks,
Martyondrums
-
maybe in about 20 or 30 years time we will have a new updated Mach3Turn
A new version of lathe, devoid of all problems and loaded with functionality, will be available in a week or so. :)
I would also like to mention that I have a bridge for sale that spans the ocean of your choice. :D
Feel free to request information at the front desk. ???
RICH
-
maybe in about 20 or 30 years time we will have a new updated Mach3Turn
A new version of lathe, devoid of all problems...
RICH
Yabbut, then what would Hood do on those long, cold Scottish nights without us'ns to baby sit?
-
I would be having fun doing CSS ;)
Hood
-
Well Hood,
I got the lathe Running perfectly. I did change to ver 57. That helped the selection of the tool in the DRO issue like you said it would do. I was not doing the right procedure for setting up offsets. Once I followed your video, everything fell into place. I am able to make my parts with 5 tools including a thread operation for the last tool. Works Great!!!!! Now, you mentioned that you would be setting up a vid on how to set offsets with hard stops as the machine zero.
That is my next task, to set up hard stops for Z and X. Let me know when you have made that vid tutorial. I would be very interested in setting my machine this way. It is exactly how we do it at work with the big uns.
Thanks for you advice.
Martyondrums
-
Glad you are sorted :) shame it needs going backwards to an old version though :(
Regarding the video, it will be basically the same except I will be using home switches as my master position and setting tools up from that, its the way I do it on the big lathe. May get a chance to do a vid this weekend but not promising as I want to try and get on with some wiring on the Chiron.
Hood
-
You guys please keep this thread active & alive with your learned discussion & videos. I read every word and watch every video that comes up on the subject.
Maybe by the time I get through phartin' around with the hardware on my lathe I'll have soaked up enough tool offset info by osmosis that I can get my front & back toolholder system working. Miracles do happen....sometimes.::)
-
You guys please keep this thread active & alive with your learned discussion & videos. I read every word and watch every video that comes up on the subject.
Maybe by the time I get through phartin' around with the hardware on my lathe I'll have soaked up enough tool offset info by osmosis that I can get my front & back toolholder system working. Miracles do happen....sometimes.::)
;D
Brett
-
Do the offsets on tool one reflect the distance from machine zero or are they still all zeros?
-
The tool table reflects my offset travel in each direction. It has the actual distance loaded in the tool tables from zero.
However, if you are at the tools offset and hit that tool number, it will show zero. A bit confusing, but it makes sense. Stay at your main tools zero and then pull up different tool numbers. You should see the offsets appear in the DRO's.
-
If setting up without home switches and using tool 1 as your master tool then machine coords can basically be anything. If you have home switches and use the home switches as machine coords zero then all tools will be offset from them.
Hood
-
So what you are saying, if the machine is set up to bump the hard switches and set the X and Y to Zero, then all my offets (even tool 1) will show distances from the zero points to the touch off points. Not like now where Tool #1 is all zeros. This will be represendted in the X and Y boxes in the offset page correct. If this is true, why can't the samethng be done with tool #1 even with out the switches? Is there something that happens when you tell mach to use auto home? Is that treated differently? I tried setting my home positions the same as my machine positions and still needed to set tool#1 offsets to zero on the offset screen. I guess I will have to set up switches today and try it. Have a good weekend.
Marty
-
I haven't setup any switches on mine other than Estop.
You would really have to have some accurate switches in order to set it up as precisely as the tool zero. I fire mine up in the morning and zero to the tool zero. By the end of the day, its still within tolerances for my parts. Not so sure that would be the case if I used home switches.
-
On my mini mill, The switches repeat very well. I start it up and home the axis' and when i go to G54 zero from the machine zero i am always within .0005".
So I am thinking it will be the same with my lathe. I give it a go and see what happens. I know at work we use the hard stops all the time and the repeat perfectly. And, all they are is micro switches mounted to the bed and slides. I hope I get the same results, it will make setup of tools much easier.
I'll post my results when I do this.
Marty
-
Approaching those stops slowly will likely help with accuracy, but go at them a bit too fast and that is where the discrepancies normally appear.
Mach has a slow down function when approaching a switch, which is nice.
-
This is exactly what I use and your right, it is a nice function for repeatablity.
On another note, Does anyone know where to find the mach3 G76 codes. I used the threading wizard and it posts out the long hand. I would like to know what the different letters on the line apply to so I can manully edit them. I know most of them, but there are I few I do not recoqnize. Any table in mach3 to explain them?. In the meantime I will chech my Fanuc manual.
Marty
-
The Turn manual has the G76 info, heres a screenshot from it, there ismore detailed info in the manual for each word.
Regarding the homing, that sets machine coords to zero so if you then jog a tool and set the offsets in relation to the switches then the home position is used instead of the master tool and thus you dont have to worry abouyt changing out inserts making other tools slightly different.
Hood
-
Old thread I know.
I am trying to learn how to modify my posts in Dolphin Cam for Turn.
One thing I need to do is to keep the spindle running during tool changes. It is gang tooling on there and someone might think the program is over. I want to eliminate that threat. There is no need to stop it until the program ends. I know Hood has helped me tremendously earlier in this thread.
I would like to do it myself. I am considering an updated version of Dcam and it says my older posts the Hood modified will not work without some modification to update it.
Thanks in advance for any help.
Lee
-
Its been a while since I dipped into the Dolphin PP but I will have a look and see.
In fact I think I have V11 unistalled on this computer, will re-install in a bit.
Hood
-
Thanks, Hood.
I have modified posts for mill before, but there seems to be more canned cycles or subroutines in turn that I am not familiar with.
Also it seems I was able to update the PP file by adding that it was version 11. ;). Surely it can't be that simple.
-
Ok had a quick look and think this is the bit you want to change
:SELCTL = {
set $CYCLETIME = $CYCLETIME + 0.5 ; 30 seconds for a tool change
#N (M09_) EOB
#N "G00"" " $YSAFPOS:YAXIS $XSAFPOS:XAXIS (M05_) EOB
Just remove the (M05_)
Regarding the PP, think the V11 one will work ok, seems to for me in the demo anyway.
Hood
-
Thanks, Hood. I don't have an M05 there. Here is that section of the post.
:SELCTL = {
set $CYCLETIME = $CYCLETIME + 0.5 ; 30 seconds for a tool change
#N (M09_) EOB
#N "G0"" " $XTLOAD2:XAXIS EOB
#N (G49_) EOB
#N " ( " $JOBTEXT " )" EOB
#N (M06_) $TOOLNO:TOOL $TLCNO:TLC EOB
}
-
Can you attach your pp and I will have a look.
Hood
-
Here it is.
http://thesharkguard.com/T_Mach%203%20Leeway%201%20test.txt (http://thesharkguard.com/T_Mach%203%20Leeway%201%20test.txt)
-
Ok just poroduced code with your PP and the only M5 I get is at the end.
You sure its not Mach that is stopping the spindle?
What option have you got chosen in General Confiig for toolchange.
What is in your M6start and m6end macros?
Hood
-
It is set for auto tool change, which it does.
Here are the macro contents.
m6start =
tool = GetSelectedTool()
SetCurrentTool( tool )
m6end =
REM nothing here in lathe
-
This is a strange one as the code I got from your PP certainly didnt have M5's in it at tool changes, does yours?
You are not using a Mill screenset by any chance?, in other words does the screenset you use have a .set or a .lset extension?
Hood
-
Just regular old Mach 3 Turn with the Blue screen set. It is an Lset. The only thing that has changed was this PP recently from the last PP that you gave me.
No I did not modify it in Notepad like I should have, but used the PP Utility provided by Dolphin.
That may be where I messed up.
On a side note, Dolphin has not answered my quote request. Each time you install a Demo, it over wrote my original version 10 or the last Demo. Tried re installing V10 and now my activation code is too old and it will not let me verify the installation unless I contact Dolphin and beg them for a reset.
Well, if they aren't interested in selling me a new version, how long will it take for them to do something with software they sold 7 years ago?
I understand the need for such security, but why does new Demo software over write my old verified software.
All these issues will help me determine what I end up getting. ;)
Thanks Hood.
-
Lets hold the phone, which is what I should have done before. They did leave me a voicemail yesterday.
I called them up and everything is okay now. :)
Maybe not with the posts, but I will post my results here.
I did decide to update to the latest version. There was a problem with the version 10, but I decided to eliminate that problem with the authentication process. Version 11 forward no longer uses a third party to authenticate the software. An email or phone call is all that is needed from V11 forward.
I'll let you guys know how it works out. Thanks a bunch, Hood.
-
Here is the Version 13 of the last post that you gave me, Hood.
I had to send it in and they updated it for me. Works great now.
http://thesharkguard.com/T_Mach3RadToolZonly4_V13.ppr (http://thesharkguard.com/T_Mach3RadToolZonly4_V13.ppr)
http://thesharkguard.com/T_Mach3RadToolZonly4_V13.ppx (http://thesharkguard.com/T_Mach3RadToolZonly4_V13.ppx)
Everything seems to be working okay in simulation. 2D sim that is. I still have a glitch in 3D sim, but they are working on that.
I'll let you know how the lathe runs.
I did do a compare on the two text files of the Posts. They only changed a few things, but those were important things. :)
-
Just to go back to the spindle issue, does your G Code have M5's in it at the toolchanges? When I used your PP it didn't, the only one being at the end of the file.
Hood
-
That is all there is in there now as well.
Now the code wants to fluctuate the spindle rather than stop it. Kind of like it is wanting to do constant surface speed rather than set spindle speed. That isn't as bad. It shouldn't be doing that either though. I'll look closer at it when I get a chance. Gotta get some parts turned out first. :)
Thanks Hood.
That new 3D simulation in Dolphin is pretty cool. Check it out if you haven't seen it yet.
There are a few videos on Youtube in the Dolphin channel.
-
Ok can you attach some code for me to look through, maybe I can see something there.
Yes the sim is the module works similar to what BobCAD, and others use.
Hood
-
;(Front Bushings .5625 Brass)
N20 G20 G18 G64 G80 G90 M49 G40 G49
; TOOL definition
N40 M09
N50 G0 Z1.0
N60 ( Twist Drill / Center Drill 0.1875" Dia )
N70 M06 T0202
N80 G97 S3000
N90 M03 G94 F15.0
N100 G40
N110 G00 X0.0 Z0.05
N120 G01 X0.0 Z-0.085
N130 G00 X0.0 Z0.05
; TOOL definition
N150 G0 Z1.0
N160 ( Twist Drill / Center Drill 0.25" Dia )
N170 M06 T0303
N180 G97 S3000
N190 G94
N200 X0.0 Z0.05
N210 G01 X0.0 Z-0.0552 F12.0
N220 G00 X0.0 Z0.05
N230 X0.0 Z-0.0052
N240 G01 X0.0 Z-0.1104
N250 G00 X0.0 Z0.05
N260 X0.0 Z-0.0604
N270 G01 X0.0 Z-0.1656
N280 G00 X0.0 Z0.05
N290 X0.0 Z-0.1156
N300 G01 X0.0 Z-0.2208
N310 G00 X0.0 Z0.05
N320 X0.0 Z-0.1708
N330 G01 X0.0 Z-0.276
N340 G00 X0.0 Z0.05
N350 X0.0 Z-0.226
N360 G01 X0.0 Z-0.3313
N370 G00 X0.0 Z0.05
N380 X0.0 Z-0.2813
N390 G01 X0.0 Z-0.3865
N400 G00 X0.0 Z0.05
N410 X0.0 Z-0.3365
N420 G01 X0.0 Z-0.4417
N430 G00 X0.0 Z0.05
N440 X0.0 Z-0.3917
N450 G01 X0.0 Z-0.4969
N460 G00 X0.0 Z0.05
N470 X0.0 Z-0.4469
N480 G01 X0.0 Z-0.5521
N490 G00 X0.0 Z0.05
N500 X0.0 Z-0.5021
N510 G01 X0.0 Z-0.6073
N520 G00 X0.0 Z0.05
N530 X0.0 Z-0.5573
N540 G01 X0.0 Z-0.6625
N550 G00 X0.0 Z0.05
; TOOL definition
N570 G0 Z1.0
N580 ( Grooving tool / Partoff blade )
N590 M06 T0404
N600 G97 S2200
N610 G94
N620 X0.2889 Z0.002
N630 G01 X0.2593 Z0.002 F8.0
N640 X0.2593 Z-0.245
N650 X0.2609 Z-0.245
N660 G02 X0.286 Z-0.2701 I0.2609 K-0.2701
N670 G01 X0.286 Z-0.3401
N680 X0.286 Z-0.4024
N690 G02 X0.2609 Z-0.4275 I0.2609 K-0.4024
N700 G01 X0.2593 Z-0.4275
N710 X0.2593 Z-0.8275
N720 X0.2609 Z-0.8275
N730 G02 X0.286 Z-0.8526 I0.2609 K-0.8526
N740 G01 X0.286 Z-0.9194
N750 X0.286 Z-0.9817
N760 G02 X0.2609 Z-1.0068 I0.2609 K-0.9817
N770 G01 X0.2593 Z-1.0068
N780 X0.2593 Z-1.1655
N790 X0.2889 Z-1.1655
N800 G00 X0.3389 Z-1.1655
N810 X0.3389 Z0.002
N820 G01 X0.2297 Z0.002
N830 X0.2297 Z-0.245
N840 X0.2609 Z-0.245
N850 G02 X0.286 Z-0.2701 I0.2609 K-0.2701
N860 G01 X0.286 Z-0.3401
N870 X0.286 Z-0.4024
N880 G02 X0.2609 Z-0.4275 I0.2609 K-0.4024
N890 G01 X0.2297 Z-0.4275
N900 X0.2297 Z-0.8275
N910 X0.2609 Z-0.8275
N920 G02 X0.286 Z-0.8526 I0.2609 K-0.8526
N930 G01 X0.286 Z-0.9194
N940 X0.286 Z-0.9817
N950 G02 X0.2609 Z-1.0068 I0.2609 K-0.9817
N960 G01 X0.2297 Z-1.0068
N970 X0.2297 Z-1.1655
N980 X0.2593 Z-1.1655
N990 G00 X0.336 Z-1.1655
N1000 X0.336 Z0.002
N1010 G01 X0.2001 Z0.002
N1020 X0.2001 Z-0.245
N1030 X0.2609 Z-0.245
N1040 G02 X0.286 Z-0.2701 I0.2609 K-0.2701
N1050 G01 X0.286 Z-0.3401
N1060 X0.286 Z-0.4024
N1070 G02 X0.2609 Z-0.4275 I0.2609 K-0.4024
N1080 G01 X0.2001 Z-0.4275
N1090 X0.2001 Z-0.8275
N1100 X0.2609 Z-0.8275
N1110 G02 X0.286 Z-0.8526 I0.2609 K-0.8526
N1120 G01 X0.286 Z-0.9194
N1130 X0.286 Z-0.9817
N1140 G02 X0.2609 Z-1.0068 I0.2609 K-0.9817
N1150 G01 X0.2001 Z-1.0068
N1160 X0.2001 Z-1.1655
N1170 X0.2297 Z-1.1655
N1180 G00 X0.336 Z-1.1655
N1190 X0.336 Z0.002
N1200 G01 X0.1706 Z0.002
N1210 G02 X0.171 Z-0.0001 I0.1659 K-0.0001
N1220 G01 X0.171 Z-0.245
N1230 X0.2609 Z-0.245
N1240 G02 X0.286 Z-0.2701 I0.2609 K-0.2701
N1250 G01 X0.286 Z-0.3401
N1260 X0.286 Z-0.4024
N1270 G02 X0.2609 Z-0.4275 I0.2609 K-0.4024
N1280 G01 X0.171 Z-0.4275
N1290 X0.171 Z-0.8275
N1300 X0.2609 Z-0.8275
N1310 G02 X0.286 Z-0.8526 I0.2609 K-0.8526
N1320 G01 X0.286 Z-0.9194
N1330 X0.286 Z-0.9817
N1340 G02 X0.2609 Z-1.0068 I0.2609 K-0.9817
N1350 G01 X0.171 Z-1.0068
N1360 X0.171 Z-1.1026
N1370 X0.171 Z-1.1649
N1380 G02 X0.171 Z-1.1655 I0.1659 K-1.1649
N1390 G01 X0.2001 Z-1.1655
N1400 G00 X0.336 Z-1.1655
N1410 X0.2889 Z-1.1655
N1420 X0.2889 Z0.002
N1430 X0.287 Z0.0009
N1440 G01 X0.1664 Z0.0009
N1450 X0.1664 Z-0.25
N1460 X0.2609 Z-0.25
N1470 G02 X0.281 Z-0.2701 I0.2609 K-0.2701
N1480 G01 X0.281 Z-0.3401
N1490 X0.281 Z-0.4024
N1500 G02 X0.2609 Z-0.4225 I0.2609 K-0.4024
N1510 G01 X0.1664 Z-0.4225
N1520 X0.1664 Z-0.8325
N1530 X0.2609 Z-0.8325
N1540 G02 X0.281 Z-0.8526 I0.2609 K-0.8526
N1550 G01 X0.281 Z-0.9194
N1560 X0.281 Z-0.9817
N1570 G02 X0.2609 Z-1.0018 I0.2609 K-0.9817
N1580 G01 X0.1664 Z-1.0018
N1590 X0.1664 Z-1.1655
N1600 G00 X0.331 Z-1.1655
N1610 X0.287 Z-1.1655
N1620 X0.287 Z0.0009
N1630 G97 S2200
N1640 G94
N1650 X0.331 Z0.0009
N1660 X0.331 Z-0.5825
N1670 G01 X0.0 Z-0.5825 F6.0
N1680 G00 X0.331 Z-0.5825
; TOOL definition
N1700 G0 Z1.0
N1710 ( Twist Drill / Center Drill 0.25" Dia )
N1720 M06 T0303
N1730 G97 S3000
N1740 G94
N1750 X0.0 Z-0.5325
N1760 G01 X0.0 Z-0.6377 F10.0
N1770 G00 X0.0 Z-0.5325
N1780 X0.0 Z-0.5877
N1790 G01 X0.0 Z-0.6929
N1800 G00 X0.0 Z-0.5325
N1810 X0.0 Z-0.6429
N1820 G01 X0.0 Z-0.7481
N1830 G00 X0.0 Z-0.5325
N1840 X0.0 Z-0.6981
N1850 G01 X0.0 Z-0.8033
N1860 G00 X0.0 Z-0.5325
N1870 X0.0 Z-0.7533
N1880 G01 X0.0 Z-0.8585
N1890 G00 X0.0 Z-0.5325
N1900 X0.0 Z-0.8085
N1910 G01 X0.0 Z-0.9138
N1920 G00 X0.0 Z-0.5325
N1930 X0.0 Z-0.8638
N1940 G01 X0.0 Z-0.969
N1950 G00 X0.0 Z-0.5325
N1960 X0.0 Z-0.919
N1970 G01 X0.0 Z-1.0242
N1980 G00 X0.0 Z-0.5325
N1990 X0.0 Z-0.9742
N2000 G01 X0.0 Z-1.0794
N2010 G00 X0.0 Z-0.5325
N2020 X0.0 Z-1.0294
N2030 G01 X0.0 Z-1.1346
N2040 G00 X0.0 Z-0.5325
N2050 X0.0 Z-1.0846
N2060 G01 X0.0 Z-1.1898
N2070 G00 X0.0 Z-0.5325
N2080 X0.0 Z-1.1398
N2090 G01 X0.0 Z-1.245
N2100 G00 X0.0 Z-0.5325
; TOOL definition
N2120 G0 Z1.0
N2130 ( Grooving tool / Partoff blade )
N2140 M06 T0404
N2150 G97 S2200
N2160 G94
N2170 X0.331 Z1.0
N2180 X0.331 Z-1.165
N2190 G01 X0.0 Z-1.165 F6.0
N2200 G00 X0.331 Z-1.165
N2210 X0.331 Z0.0
N2220 X0.0 Z0.0
N2230 M05 M30
-
There is nothing in the code, that I can see anyway, that will fluctuate the spindle RPM. The calls are G97 which is Revs per Minute, so no CSS calls at all.
Hood
-
That was my conclusion as well. It may be noise in the motor controller. I don't normally run the lathe. My Son and his Wife does. They probably would not realize the spindle is acting differently.
I am considering putting a servo motor on it instead of the DC motor that is on there now.
Much better control of the spindle speed that way as well as direction then. It could finally be able to do some threading.
I used to take care of threading with a little 7/14 manual lathe. That motor control burnt out, so it isn't running.
I think I would much rather do cnc threads instead. ;)
Judging from the time it took my mill to burn through the brushes on it's old DC motor (similar) then this one is getting close to needing replacements sourced anyway.
I had always intended to do threading eventually, so it is about that time.
Servo's are relatively new to me so I'll have to research them a bit. Any recommendations? :)
-
You can thread with any motor as long as it is powerful enough and relatively steady in RPM. Sounds however like you may be needing new brushes in it, so if you fix them you should manage threading fine.
Regarding servos, well I just pick mine up on eBay so cant really recommend any. One warning, if its AC servo then it is best to make sure the motor and drive are a pair as AC servo drives often can not be set up with motors they are not intended for.
Hood
-
I did buy the spindle encoder that uses a hole in a disk, but never installed it. It is partially a trust issue I think. I think I would trust a servo setup more and it would be more precise than the motor I have on it now.
It doesn't have any braking on it.
I am currently running the steppers off of Gecko 203V's. 72 VDC 12 Amp PS. The lathe is only 110 VAC right now, but it sits close to the circuit panel and I could runn 220 to it as well to run a spindle from. My question now is if I did use a 220 VAC and chose AC servo's, could it use the same BOB as the DC steppers? Right now, the motor controls are inside the control panel on the larthe.
(http://www.cnczone.com/forums/attachment.php?attachmentid=73338&d=1231677075)
There is a need now to find an answer before my little motors quits completely, but I haven't decided to go with servo's yet. I was unable to locate brushes for my old mill motor, but I may be able to find them for this one. That would give me more time. :)
-
You dont need braking for threading on a lathe as the spindle never halts from pass to pass.
Are you talking about rigid tapping instead of threading? If so then Mach does not natively support rigid tapping, it can be done with some external controllers however.
If you have a servo spindle then you can do rigid tapping with Mach via the parallel port but it is a work around and requires SwapAxis()
Regarding the BOB, yes as long as the drive is capable of Step/Dir command then it will work from the same drive. Most industrial servos prefer differential Step/Dir signals although most can be connected single ended. It is however easy enough to put a line driver on the Step/Dir output of the BOB to give differential signals and would be the preferred option.
Hood
-
Right. I was thinking rigid tapping. Not having done threading on a cnc lathe, I confused myself with it. ;)
Spindle keeps turning the same direction for use with a threading tool.
I will try to do a CAM part that maintains one speed throughout and see how the spindle reacts.
It is still stopping and starting, but never gets a chance to stop completely.
The Check box for CSS in not lit in Mach 3, but it does flash numbers beside it when it's running and those do change.
Honestly I have never really noticed those before. :(
-
I dont use the standard Turn screen so afraid I ave no idea weter te CSS DRO sould display numbers or not.
Hood
-
Thanks, Hood.
Definitely something still going on with it. I'll investigate further and let you know if I get it sorted out. :)
-
Well,I ran some of the old code output by V10 and it used your unmodified PP that you gave me earlier in this thread.
The spindle acts exactly as it should in that file. It regulates to initial speed and then continues steadily during that operation. Changes to the next called speed on the next op. This is as it should be.
V13 is definitely doing something different.
I thought it might had been a Mach 3 settings somewhere, but nope.
I will compare texts files and see what the difference actually is. I'll then post the results here.
-
Not sure how that could be as the code you showed didnt have a G96 in it and that is the only way I can think of that the spindle speed could vary whilst cutting.
Look forward to what you find out.
Hood