Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: natefoerg on December 12, 2012, 12:31:05 AM
-
I have been loosing my mind trying to get Mach3 to run a lathe program as I intend it to.
Some basics-
Retrofit Hardinge CHNC1 running steppers, SmoothStepper, G203V's.
No toolchanger. Running Gang tooling on a tooling bar at 1.000" centers (Omni turn style)
I have the gang tool bar set up like this-
1st position. master tool holder. tool 1.
2nd position. NO TOOL. BLANK.
3rd position. tool number 2.
4th position. tool number 3.
5th position. tool number 4.
NOTE: 1st position is closest to operator.
I have a relatively simple file I created in BobCad ver 25 lathe that has the following-
1 spot drill op. done with tool 2, a spot drill in the 3rd bar hole.
1 through drill op. done with tool 3, a jobber length drill in the 4th bar hole.
1 roughing/finishing profile op. done with tool 1, a cutoff style tool in the 1st (master tool) bar hole.
1 cutoff op. also done with tool 1.
1 chamfer in prep for bar pull, done with tool 1 also.
1 bar pull done with a puller, tool 4, in 5th bar hole.
Loop.
I know that my locations of tools 2,3 & 4 are 1 inch apart from each other and they are tools that do not use an X offset (because they are drills and a bar puller.)
I know that tool 1 (master tool) is not on a center and is at an arbritrary place.
If my stock is .5" dia, and I want to setup the master tool, and then the others how do I go about this?
I have RTFM like 10 times and have been trying things for hours...
I suspect that this is all so much simpler than it seems. but with several diff coordinate systems, offsets, touch offs, entering cut diameters in the X axis DRO, Etc. I am so confused...
Can someone lay it out from start to finish?
Note-
I have used G52 to run this part in the past, but I think this is less than ideal on a ton of levels. for instance- wear offsets. also- I am calling a tool, but not really. more like I pretend to call a tool and just shift the part location. Seems wrong to do that.
-
I never use work offsets (other than the G54 ) as I have never seen a need.
My lathe screen is totally different from the standard lathe screen but here is what I do.
I home the machine then call Tool 1
I then move tool 1 in to take a light cut and just before the cut I zero the X DRO or set it to close to what I think the Dia will be. This is so I can MDI the cut, move out on X then clear on Z and back in to X again. I then measure the Dia and on then enter that number in the (What the standard screen calls) Part Zero Coords DRO. I then press Touch X button and you should see the X DRO reflect that your tool is at that Dia. It is best to then open the tool table press apply then exit, (my Touch X and Z buttons automatically open the table for me)
Next do the same with the Z, ie move to just negative of the end of stock and zero the Z Dro then take a light cut, no need to touch off Z for this one.
Now jog away and call Tool 2, repeat as above for X or alternatively just use a feeler to touch off on Dia, enter the Dia in the X part zero coords DRO (remembering to add feeler thickness to Dia, 2x feeler thickness if in Dia mode) Then as above press Touch X, open Tool table and save. Next move Z to touch end of stock, enter zero in the Z Part Zero DRO (or if using a feeler enter the thickness of it) and then press Touch Z, open table and apply.
Repeat for the rest of your tools, remembering to call a new tool before you set it up.
The above assumes you have accurate home switches if you are wanting to start your machine and know the tools wil be the same position as the previous day.
For doing the actual touch offs I have made up a tool for the chuck that I can take a light skim cut of with tool 1 then any other tools I want to set I just move to touch off dia and end and a LED tells me when I am there and I can then set the tools as above. Its just a bit easier than the feeler method, especially as my tools are at the rear of the work and the lathe is big so I cant really see where the tools are in relation to the work.
Hood
-
Just to add for drills etc you can use the same method for X by touching off the dia but you have to remember to take the half the drills Dia into your value for the X Part Zero DRO value.
Hood
-
Just a quick comment nateforeg,
Do exactly what Hood said and do it three times correctly (to form a habit of doing it right). The problem is one is so focused on trying
to touch off the tool that that you forget to call a different tool or click on one of the buttons, etc and
don't realise it.
RICH
-
If Lupe parked on the 50 yard line. Never mind I didn't understand it either when setting it up the first time. I am still vague though I do get it right eventually. IIRC don't you use the "ref" for the first or master tool and then just save for all the rest of the tools?
-
It can be done all sorts of ways and depends on whether you have accurate home switches or not or even none.
I tend to have Tool 1 with zero offsets and I have a Home Off value in my homing and limits page for the X which will represent the Dia that Tool 1 is when homed.
Another option is like I describe above, setting an X offset for Tool 1 which is an offset referenced to your home position.
There are many more ways but that is the easiest two ways in my mind.
Hood
-
Hey Nate, see if this helps http://www.cjh.com.au/Gang%20Tool%20Block%20Offsets%20for%20CNC%20Lathes%20under%20Mach3%20Control.pdf Kind Mr. Chris Humphris did a fantastic job of documenting the process that works for him.
I'm getting close to setting tool tables up on my ORAC retro and RTFM'ing and searching on the forum still has me dazed. I printed the sections in the manual that deal with homing & tool tables/offsets and I read it during lunch at work almost every day. I guess I'll try wadding the pages up and eating them next. Maybe that'll work. ;D
-
DB-
Thats actually the way I have run the prog in the past. It works, but is not simple and I imagine that it should be easier to just use mach 3 tool offsets as designed.
I never could figure out why my G52 offsets ended up being ~1.9 inches away from each other per tool, when the tool block is on 1" centers. Never made any sense....
-
Also, I should add that I am not running limit switches.
-
I don't have homing/limit switches on my other little lathe and grew tired of having to constantly reset the X-axis zero point and get it to cut consistent diameters without fiddling around a lot.
I spent the nec. time to install & config opto sensors on X & Y on the ORAC and am real happy with the repeatability of referencing on the X-axis now. It's worth the time & effort in the long run to know that it's going to cut the same dia. with the same tool each time I turn it on & re-reference it.
-
I have a few good quality switches that I can install on my machine. I should do that.
When I turn on the machine, I could home x and z and then the machine will know exactly where the cutting points of the tools are correct?
The tools would just have to be recorded in the tool offset table as the distance each one is from X0, Z0 (the homed position) does this sound correct?
Example.
Home-
Table moves to X0 about 5 inches out from centerline of spindle.
Saddle moves to Z0 about 18 inches away from spindle face.
Both positions recorded as Z0, X0.
Then, I could move the master tool over to a workpiece and touch in Z and record the travel distance as the master tool Z offset. I would then take a skim cut, measure and move the tool in in X until it was at 50% of the X number I got from the skim cut. This would put the master tool tip exactly at X0. I could then enter the X distance travelled from the X home position to the master tool tip at X0 location, into the master tool X offset box.
Then I could measure the distances from the other tools in the gang from the master tool tip's Z and X offsets and add the measurements to the master tools offset numbers and then put the total intoi each tools offset table.
This all seems to make sense to me. Is it correct? and is this doable in Mach3?
-
if the above method would work, would it make sense then that when I draw lathe parts in CAD/CAM, that I draw them at a Z(negative) position that has the part face at the distance from the Z home position that it needs to be, when it is set out from the spindle face enough for the turning ops and cutoff.
Example-
Program part in CAD/CAM with a 1.5 inch long part held out .5 for clearance from spindle face. Total material stickout would be 2" and this 2" face location from the spindle would actually be -16" from the Z home position(knowing that my spindle face is -18" from the Z home position(Z0)) .
To do this, I would draw my part with its face at Z-16" in CAD/CAM.
This making sense?
-
If you dont have home switches then you could do as described but it just means each time you start Mach you will have to take a cut with your master tool and type the dia into the X Dro, all other tools would still be correct once that was done.
Fitting switches would likely be a better option however as it would solve the problem of having to set the X every time you start Mach. When I start my lathe, home then call any tool and tell it to go to a Dia it does. For Z, that changes from job to job so the home switch is not quite so important on that although it does come in handy if ffor example you are running the same job the next day.
Hood
-
Great, so what I propose should work if I have home/limit switches installed?
Additionally, does drawing the parts in cad at the -Z location as I described make sense?
I think I might be getting a bit closer to understanding this...
-
I have a few good quality switches that I can install on my machine. I should do that.
When I turn on the machine, I could home x and z and then the machine will know exactly where the cutting points of the tools are correct?
Definite yes IMO on the switch issue although I'd go with optos instead of mechanical at least on the X. I went through 3 (what I thought were) "good quality" mechanical switches before getting one that was reasonably consistent.
Yes on statement 2 except the machine will know exactly where your SWITCHES are but won't know where the tool tips are until you set them up. That's where my knowledge ends as of this time. I'm still trying to get my head around the tool table and offsets. I have established where the spindle center is via cutting a piece of stock, measuring the dia. and using that to MDI to the center and then zeroing the X DRO. Works great for that tool but will have to set up the table for other tools before it becomes really useful.
edit: oops, Hood posted before I could type this so dunno if this helps or not.
I'm slow but I'm old so I have somewhat of an excuse.;)
-
Personally I wouldnt have Z the same on all parts but if all your parts will be of similar length then it may be ok. However to my mind it is just as easy to move close to the end of the stock and then take a facing cut and setting that as Z zero. Doesnt matter which tool you use if they are all set in the tool table as calling another tool will offset the Z for it.
Hood
-
Yeah, i was just talking about how I would draw that one particular part in CAD/CAM. It would have to be diff for each different part. Same principal though...
-
I will try and explain how I work. Z Zero is always the end of the stock and any material being removed in Z is towards the chuck, so negative. I put the stock in the chuck maybe leaving 10mm extra longer than the part, so say I was making a part that was 200mm long I would have 210mm sticking out the chuck. I would then call the tool I use for facing and move it to the end of the stock and enter 0.2mm into the Z DRO, then my first cut in the code would be a facing cut, it will move to Z Zero and face off, it will remove approx 0.2mm from my stock.
Now if the next part is 30mm long I will place that in the chuck with maybe 40mm sticking out and do the same, move Z to face of stock, enter 0.2mm into the Z DRO and again when I start the code it will face off the part.
Its kind of hard to explain, would be simple if I could take a vid of tool setup and how I work, maybe when I get the wee lathe up and running fully I can, big lathe is just too big to be able to set up a camera for that.
Hood
-
...maybe when I get the wee lathe up and running fully I can, big lathe is just too big to be able to set up a camera for that.
Yes please...show us how you set up and use your tool table too!:) You make it sound so easy and I'm sure it is once one gets "over the hump."
-
I never could figure out why my G52 offsets ended up being ~1.9 inches away from each other per tool, when the tool block is on 1" centers. Never made any sense....
I use G52s with my gang tool holder, but then mine is set up for drills only, so the X offset never changes, and I just manually edit the G-code if the drill lengths change (I have a whiteboard with a corner dedicated to the drill offsets).
As to your offset being off, now you mention it, I think there is actually a bug in the tool change macro.
I noticed that if after doing a tool change where the X offset changed alot with minimal Z movement, the X axis would loose lots of steps/stall. It's like Mach was ignoring the X axis maximum speed, and setting speeds via the Z axis settings.
For example, if the X-axis had to move 80mm and the Y only 10mm, it would move the Y at rapid speed, and X would stall as it was expected to move at speeds far higher than it should.
I worked around it by adding extra lines to the G-code that move the carriage into the approximate place that is needed after the tool change.
I suspect the issue is something in the tool change macro, however I've never had a chance to look into it in any more detail, and given how cold it is outside, I'm taking the "if it's working, it doesn't need fixed" approach!
-
I have installed the X and Z limit switches on my machine this evening. I have not wired them in yet, but the hardware portion is done.
-
Got them wired in and lighting up the "led" on the diagnostics page.
Now I have to figure out how to instruct mach to home the axes.
-
A bit of progress. I found that g28 will send the machine to Z home (+14.000) and then X home (+4.000) Seems odd that Z homes first. Seems it should home X first for clearance and then Z. Is there a way to change this?
Also- I thought that I should be able to just press the "home all" button and it would home itself. Cant seem to figure that out...
Note, although switches and wiring are done, and I know they are functional. I am not runnning these tests on the machine. I am trying to figure out homing out of the shop (in the basment) because its bedtime here and I am just running mach on a laptop...
-
...maybe when I get the wee lathe up and running fully I can, big lathe is just too big to be able to set up a camera for that.
Yes please...show us how you set up and use your tool table too!:) You make it sound so easy and I'm sure it is once one gets "over the hump."
I will see if I can mock up something on the wee lathe as tools and make a quick video. I only have one holder for the toolpost so cant use that and I also only have a threading tool small enough to fit in the holder anyway. I should be able to make up some sort of gang tool mock up in the next few days and try and make a video.
Hood
-
I never could figure out why my G52 offsets ended up being ~1.9 inches away from each other per tool, when the tool block is on 1" centers. Never made any sense....
I use G52s with my gang tool holder, but then mine is set up for drills only, so the X offset never changes, and I just manually edit the G-code if the drill lengths change (I have a whiteboard with a corner dedicated to the drill offsets).
As to your offset being off, now you mention it, I think there is actually a bug in the tool change macro.
I noticed that if after doing a tool change where the X offset changed alot with minimal Z movement, the X axis would loose lots of steps/stall. It's like Mach was ignoring the X axis maximum speed, and setting speeds via the Z axis settings.
For example, if the X-axis had to move 80mm and the Y only 10mm, it would move the Y at rapid speed, and X would stall as it was expected to move at speeds far higher than it should.
I worked around it by adding extra lines to the G-code that move the carriage into the approximate place that is needed after the tool change.
I suspect the issue is something in the tool change macro, however I've never had a chance to look into it in any more detail, and given how cold it is outside, I'm taking the "if it's working, it doesn't need fixed" approach!
I am wondering how you are doing things when you say you think its the macro. If using offsets are they all in your code? If they are then I would imagine you have Mach set to Ignore Tool Changes. Is that the case? If it is then the M6start macro will not be used at all. Maybe you have the offsets in your macro instead and have it set to Auto Toolchange?
Hood
-
A bit of progress. I found that g28 will send the machine to Z home (+14.000) and then X home (+4.000) Seems odd that Z homes first. Seems it should home X first for clearance and then Z. Is there a way to change this?
Also- I thought that I should be able to just press the "home all" button and it would home itself. Cant seem to figure that out...
Note, although switches and wiring are done, and I know they are functional. I am not runnning these tests on the machine. I am trying to figure out homing out of the shop (in the basment) because its bedtime here and I am just running mach on a laptop...
The guy that made up the lathe screenset a few years back didnt reckon homing was much use on a lathe and that is probably why it doesnt act like most expect it should. It is also one of the reasons I made up my own screenset after about 2mins of trying to use the lathe screenset. Easiest thing to do would be to open the screenset with Screen4 or MachScreen and change the HomeAll button to a VB button then save as a new named screenset. Open Mach and load the new screenset and then go to operator menu then to Edit Button scripts and the HomeAll button will be flashing. You can then click it and in the editor window you can paste the following, that will home X then Z, personally I prefer Z then X but its just my preference.
DoButton(22)
DoButton(24)
Hood
-
I am wondering how you are doing things when you say you think its the macro. If using offsets are they all in your code? If they are then I would imagine you have Mach set to Ignore Tool Changes. Is that the case? If it is then the M6start macro will not be used at all. Maybe you have the offsets in your macro instead and have it set to Auto Toolchange?
Hood
I still use manual tool changes with a QCTP, as it's only the drills that are ganged.
One of the reasons I use G52 is to avoid having to click start between drills.
I'm sure there is a better way to do things.
-
Ok! I made a bit more progress.
First- G28 does not stop on a home switch for me. it just kept going...
But, I now have Mach3 homing the Z and X (manually) by pressing "set home Z" and "set home X"
This works, but I would have thought "home Z" and "Home X" would have been the correct commands....
Anyway, is their a way to go in and change the rate at which the machine travels to home Z and Home X? My machine only has max 30IPM, and it appears that when using "set home Z" and "set home X" that it only wants to travel at .29IPM! painfully slow! Sure I can jog over to a better spot and start from there, but I would rather just hit the buttons and have it travel over at 10IPM.
Does it make sense that I maight write a macro that I can assign the "home all" button to, that will home X at 10IPM and then home Z at 10IPM? Also, could this macro be written to then assign a number to the home locations IE: Z 4.00 and X 16.00?
Mabie this is what the G28 "home location coordinates" are for? or mabie not, I have not been able to use G28 sucessfully. It seems that when I do G28, that it just goes to the numbers I have put into the "home location coordinates" boxes, and does not stop at the actuation of the switches and then re write the home locations to be the numbers in the "home location coodinates" box, like I thought it would have.
So many questions...
-
Under Config, Homing/Limits, set the % of G0 speed at the far right.
Russ
-
Excellent info Overloaded!
I can home at 100% on this machine because the max IPM is 30. The machine has a 5:1 ratio by design. I believe they wanted high res and decent speed with the original servos.
-
I am wondering how you are doing things when you say you think its the macro. If using offsets are they all in your code? If they are then I would imagine you have Mach set to Ignore Tool Changes. Is that the case? If it is then the M6start macro will not be used at all. Maybe you have the offsets in your macro instead and have it set to Auto Toolchange?
Hood
I still use manual tool changes with a QCTP, as it's only the drills that are ganged.
One of the reasons I use G52 is to avoid having to click start between drills.
I'm sure there is a better way to do things.
Ok I see what you are meaning now, you are using both tool calls and G52's in the same code dependant on which tools are being used.
Best way is to just set the tool table up and forget the G52's
Hood
-
Ok! I made a bit more progress.
First- G28 does not stop on a home switch for me. it just kept going...
G28 sends Mach to the Home position, if you have not homed then Mach may think your home position is further than it actually is :)
But, I now have Mach3 homing the Z and X (manually) by pressing "set home Z" and "set home X"
This works, but I would have thought "home Z" and "Home X" would have been the correct commands....
As mentioned earlier the screenset is a bit weird when it comes to things like homing ;D
Also, could this macro be written to then assign a number to the home locations IE: Z 4.00 and X 16.00?
If you are meaning to set the Machine Coords at something other than zero when you have homed then you do that by entering a value in the Home Off box on Homing and limits page.
-
Ok I see what you are meaning now, you are using both tool calls and G52's in the same code dependant on which tools are being used.
Best way is to just set the tool table up and forget the G52's
Hood
Will that not mean the lathe will stop and wait for a toolchange between drills?
-
The way I would get around that is have it on Auto and have the macro look at the tool being called, if its a tool thats on the QC post then have it turn off the spindle and and then exit the macro. You could then change the tool and press Start. If the tool being called was a drill then you could have the macro just continue the code.
Hood
-
Update-
I now have the limit switches installed/wired and working.
When I "set home X" the machine goes to home in X, steps back off the switch and records the position that is entered in the "home off" box. Same for Z. This is much of what I have wanted to accomplish!
Now I need to figure out how to record the offsets for each tool in the gang bar.
-
Do it by touching off each tool to a piece in the chuck of a known diameter.
-
...maybe when I get the wee lathe up and running fully I can, big lathe is just too big to be able to set up a camera for that.
Yes please...show us how you set up and use your tool table too!:) You make it sound so easy and I'm sure it is once one gets "over the hump."
Video showing one method of setting lathe tools in Mach, it is a bit wobbly I am afraid but hopefully it will help to show how easy it is.
http://youtu.be/mWnfioI3G0E
In this video the lathe doesnt have home switches so I will set tool 1 X and Y coords but have zero offset in the tool table. When I start Mach I would just take a light skim of the face and set that as Z Zero and same for the Dia but this time measure the Dia and enter that into the X DRO. Any tool called after that will be offset from these dimensions.
If you had home switches that were accurate you could use them as your "master tool" and set all tools in the tooltable in relation to the Home position rather than a master tool as I have done.
In the video I have used a device I made up for setting the tools in the big lathe, it consists of two bits of steel separated by a delrin insulator and then I have a LED and battery that I connect between the two part, when the tool contacts the front part it completes the circuit and the LED lights up.
Ok so for setting tools I take a face cut and a dia cut and can then set the rest of the tools without having to actually cut any more stock as the LED will light when I touch the part. This device is not needed as you can just take a skim cut of the Dia with each tool and measure each time and for the Z just touch off the end with a feeler but on my big lathe the tools are behind the stock so its hard to see and this just makes things easier.
Hood
-
Awesome Robin, thanks, that helps a lot! ;D
Gotta get after it the 1st weekend after New Year's Day. I'm sure I'll have more questions to ask but hopefully they'll be a lot more intelligent.
-
For you it would be easier as you have accurate homing. All you would do is home then move the first tool and take a skim off Z and then enter zero into the Z's Part zero DRO and press touch Z, Take a skim of X, measure and enter that into the X's part zero DRO and press Touch X, repeat for the rest of the tools. Your home switches would basically be taking the place of tool 1 in that video, ie they would represent the master position of which all tools would be referenced to.
Hood
-
Hi Hood,
This is a very helpful tutorial video of setting tools on a lathe. Keep seeing people asking just about that every now and then. Sure the video will help many. May be the link could be put under Members Docs section or something.
Dan
-
Dan,
Its a bit shaky and not scripted but hopefully it will help a few.
Hood
-
Have had a few people ask about the touch off tool I have in the chuck in the video, its really simple and below is a pic showing how its constructed, basically a bit steel bored out, a delrin bush as an insulator and then another piece of steel pressed into the delrin.
Hood