Machsupport Forum

Third party software and hardware support forums. => LazyTurn => Topic started by: lcvette on August 18, 2015, 06:09:23 PM

Title: Gcode Request for a part
Post by: lcvette on August 18, 2015, 06:09:23 PM
Hey guys,

I am trying to develop a post processor to use on a lathe and was wondering if anyone would mind turning a part into gcode for me so i could see what correct code output looked like..  I have been battling this for a few days and haven't  gotten it nailed down yet.  i have been able to get mach3turn to accept the file without error but the toolpath looks all wrong.

Would anyone mind making some code to help me out?

I have the part file in solidworks but could easily send it via DXF or any other format really, just want to see some solid code so i can edit the universal post generator to output the same..  I did it for my mill but I had other cam software at the time to help guide me along the way to what it was supposed to look like.. for the lathe I have bubcus..

Thanks in advance!!

Chris
Title: Re: Gcode Request for a part
Post by: RICH on August 19, 2015, 07:42:21 AM
There are a lot of wizards that can be used to generate Gcode for the lathe.
Why not use them to see  what the code looks like?

RICH
Title: Re: Gcode Request for a part
Post by: lcvette on August 19, 2015, 04:34:29 PM
was wanting to see what tool changes and such would look like as well, more like what a cam package would output for mach3.  I will dig around some more and see what i can find.

Thanks!

Chris
Title: Re: Gcode Request for a part
Post by: Hood on August 19, 2015, 05:31:45 PM
If you want I can run your model through BobCad and give you the code it produces.
Hood
Title: Re: Gcode Request for a part
Post by: lcvette on August 19, 2015, 06:27:43 PM
Hood,

that would be awesome, what format would you like and where would you like it sent?

Thank a TON!

Chris
Title: Re: Gcode Request for a part
Post by: Hood on August 20, 2015, 02:37:32 AM
Just attach it here, you may have to zip it though as the forum only accepts certain file extensions.
You could try it as the .sldprt as BobCAD can open them.
Hood
Title: Re: Gcode Request for a part
Post by: lcvette on August 20, 2015, 12:59:02 PM
Hood,

Here ya go, I attached the parts file in a zip folder.  Thank you so much for your time and effort!! hopefully I can get this post nailed down, if so I will be happy to share it!

My Best Regards!

Chris

Title: Re: Gcode Request for a part
Post by: Hood on August 20, 2015, 01:59:13 PM
Ok wasn't sure how you would do this, ie in one hit or OD then turn for ID. I did it in one hit using a round insert for the OD.
Other thing is it is in metric Dia mode as that is what I use, hopefully that won't matter for you. If it does then I will see if I have an Imperial post and re-do, not sure if I have one though.

Anyway code is attached and also a link to a youtube video showing the preview, still uploading so it will be about 10mins probably before you can view.
http://youtu.be/dGUeTm0oiAM

Hood
Title: Re: Gcode Request for a part
Post by: lcvette on August 20, 2015, 02:01:57 PM
Ok, going to see how it plays when i run it through mach!  video is set to private and wouldnt let me view..

Thanks Hood!
Title: Re: Gcode Request for a part
Post by: Hood on August 20, 2015, 02:03:43 PM
Think vid would just be loading, try again and see, if you still cant see let me know.
Hood
Title: Re: Gcode Request for a part
Post by: Hood on August 20, 2015, 02:39:57 PM
Here is a link to the actual presentation where you can download and run it. You can rotate, speed/slow etc just as you could if in BobCAD itself..

http://WDMyCloud.device2441142.wd2go.com:9093/api/1.0/rest/file_contents/Public/N54%20Charge%20Pipe%20Adapter.exe?device_user_id=15760889&request_auth_code=c291222ed591f12b51ceec6d9d5602a919e768dbaa832148abd37e838cff06a2



Hood
Title: Re: Gcode Request for a part
Post by: lcvette on August 20, 2015, 02:47:59 PM
Hood,

Saw the video, looks awesome! my simulation looks pretty much identical so it should make it as accurate as possible.  mach accepted it and ran it same as simulation so i know i have a viable starting point of how the code should look, now just need to go through all of the settings in the UPG and keep tinkering with them until they spit out the appropriate code.  You are the friggin man and I can't tell you how much I appreciate your help on this!  I wrestled the same thing while  straightening out the post for the mill, but eventually got it working flawlessly.  Unfortunately I know infinitely less about lathes and lathe code so it is a bit of a learning curve.  I am making models of all of my tool holders and inserts so it has accurate geometry to use in it tool path generation, unfortunately it doesn't have anything preloaded for tiny tools like I am using..lol

I will work on it some more tonight when i get home and see if i can make heads or tails of anything!  Again, thank you so very much for your help!

Best Regards!

Chris
Title: Re: Gcode Request for a part
Post by: Hood on August 20, 2015, 02:53:09 PM
What CAM are you making the post for, is it LazyTurn?

You can often download DXF or IGES files from the likes of Sandvik or Seco or Kenametal for your tools.
Hood
Title: Re: Gcode Request for a part
Post by: lcvette on August 20, 2015, 02:54:32 PM
that is great information, hadn't though if that!  I'm using Camworks.
Title: Re: Gcode Request for a part
Post by: Hood on August 20, 2015, 02:58:17 PM
Ah ok, never used that.
Hood
Title:
Post by: lcvette on August 23, 2015, 12:30:07 PM
I've got it outputting useable code, everything looks good with the movements, just trying to write a decent tool change command.  It has a few different areas to configure such as rapid to tool change, initial tool change, subsequent tool changes and rapid from tool change.

Alot of it is confusing because it will stop for a tool change with different codes and not necessarily an M6.

And of course it is alot of trial and error with the language and how to format it properly.  All in all I love the fact it allows me to make changes and I know I will get it there, just going to take a little tinkering on it.

What I have learned is how little I know about lathes verse milling machines.. I wrestled with code being wrong for 2 days before realizing that a rear turret is a traditional turret on a lathe, once I figured that out everything started jiving with the actual movement code.

I noticed you use an M7, any reason for that over an M6?

Being I am using a G0704 mill with the head turned 90 degrees, I don't have home or limit switches setup for the lathe so determining where to send the lathe for tool changes is odd.  Between having some control in the cam software for safe retracts and indexing positions I am wondering if I would just be better off using the cam to send the mill to a tool change position and just use the post to call for the M5, M9, and M6 and subsequent G97, M3, S word, M8..

Also when zeroing a part on a lathe I always did so at the outer edge of the stock diameter and face.  Am I to understand correctly that the tool offsets to the center handle everything else?  Haven't added a tool library yet.

I assume that the tool offsets will be handled in mach3 so I have then turned off in the cam software.  However for the tool tip, in the cam I have to set all of the tools up by the center point of the tool tip radius and set it as the 0, 0, 0 coordinate in the model.  Will this conflict with the mach tool table settings?  I am unclear if the gcode is posted with the tool tip radius taken into consideration and if so which would be the better solution to make the tool tip a point in the cam and let mach3 handle it or set it to zero in mach3 and let the cam handle it.

Any thoughts?

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on August 23, 2015, 06:11:51 PM
M7 is my coolant, I used to have a front and a rear turret so I used M7 for my rear turrets coolant and M8 for the front turret.

 M6 is for a tool change but on Mach Lathe it is not required, You can use M6 if you wish or not if you don't, I choose not to, all you need is the T****.

X0 is the centre line of the lathe, so if you take a skim cut and measure the diameter (assuming in Dia mode) then you enter that value in the tool table.
Here is a vid I did showing how to set up some tools which may help.
https://www.youtube.com/watch?v=mWnfioI3G0E

You can change a tool at any position on a lathe, often you code it so that the tool is just clear enough to not hit anything.
Hood

Title: Re: Gcode Request for a part
Post by: lcvette on August 24, 2015, 12:05:03 AM
Hood,

Thanks a million!  very informative and very helpful.  I went ahead and used the M06 call in the post because I have machstdmill/lathe and will likely use it down the road so it is nice to have all the buttons in places that are familiar..  i have not dug into it yet, but i believe it uses a tool change macro which can be setup similar to the mill profile.  for now i just used a safe retract function in the cam software that will automatically remove the tool and send it to a designated indexing position at a tool change call, currently setup for x2 z4, I will probably change the x to 2.5", i have a 4" lathe chuck and my mastertool is the longest tool in my box so it should always give me clearance for any changes i need to make, and without a tail stock, i doubt i will be turning anything over 4" long so should be good there as well.

I attached a copy of my post, I will be using a cored 2" piece of stock for these parts and I haven't yet added a cutoff tool to generate that toolpath yet, probably tomorrow.  the only tool i had was a neutral 35* diamond insert to cut the back portion of the part which is why it is creating a V.  You got me all hot and bothered about a round insert and tool holder but i haven't found any budget oriented offering for one yet, i could see that tool being VERY useful!

I really appreciate all your help, I am currently cross eyed from going through the post code, very intimidating for someone who has never programmed anything before.. just shear will was driving me on..hahaha

let me know what you think of the code, a few things that were killing me was that everytime i would put a G91.1 in the post it made things screwy.. so i ended up just setting the post to have all I,J moves output in incremental and with mach set for I, J moves to be incremental it seems to jive just fine.  i have the feed setup to call for either fpr or fpm depending on what i click in camworks, being i am unfamiliar thus far with values set in fpr and have gotten some experience from manual jog turning and using the wizards for basic turning jobs, i will probably stick with them for a while until i feel good about everything else.

you da man!

Chris
Title: Re: Gcode Request for a part
Post by: Hood on August 24, 2015, 06:12:35 AM
Did you attach the correct code? Looks like the file I attached. The .set one just seems to have the tool designations in it and noting much else. maybe it needs the CAM to open correctly? I was just using Notepad++

Regarding the feed,  much better to use G95 on a lathe  in my opinion as you will normally only use a few different feeds. For example on my big lathe I tend to use 0.25 to 0.3mm per rev for roughing and 0.15mm per rev for finishing. Altering the spindle speed for different materials and diameters will not affect the chipload. If using Feed per minute then you will have to enter different values depending on the RPM to try and keep the chipload constant.

I have been asked a lot of times when I will do the video for tool setting with home switches, I have never got round to doing it. I may not have the wee lathe for much longer and using a camera and setting tools on the big lathe is a bit more tricky, so now  I have home switches on the wee lathe I  better try and do it soon, basically it is a similar procedure but rather than having a master tool you use the home switches as the master.

Regarding tool change position, normally you let the CAM handle that as it is easily changed in CAM and means you do not waste time gong to a designated position if it is not required to move as far as that.

Hood
Title: Re: Gcode Request for a part
Post by: Hood on August 24, 2015, 06:22:16 AM
Oh and regarding the round tool I used in the simulation, it is a Seco MDT which can be used for light turning or grooving and can use 3mm round end inserts as well, quite a handy tool but quite expensive. I was going to get a Korloy MDT tool but I found a good deal on Seco insers so went with that instead.

MDT stands for Multi Direction Turning.

Here in the UK there are places that sell round insert tools for smaller lathes which are fairly cheap, here is a link to one such tool although it is a 6mm insert rather than the 3 that the seco has.
http://www.shop-apt.co.uk/apt-90-srdcn-lathe-turning-tools-for-rcmt-inserts/srdcn-1212-h06-apt-lathe-turning-tool-for-rcmt-0602-inserts.html


here is a link to a video of the Seco MDT tool

https://www.youtube.com/watch?v=cLz-uEvQatI


Hood
Title: Re: Gcode Request for a part
Post by: lcvette on August 24, 2015, 02:39:04 PM
Nice!  sorry about the upload blunder... try that one.  i double checked it and it should be good to go!
Title: Re: Gcode Request for a part
Post by: Hood on August 25, 2015, 08:27:28 AM
Looks good in Mach :)
Hood
Title:
Post by: lcvette on August 25, 2015, 09:31:37 PM
Gonna start making parts tomorrow, have 2 more tools to model up and then time to chick up some stock, cross my fingers and hit the green button..lol

Thanks for everything Hood.. I found a round tool holder from A hard I ordered but won't be here until Friday..

I did see that a few companies offer gooving tool inserts with round tips, wonder if they would be any good, definitely alot smaller the a 6mm round for getting in tight places..

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on August 26, 2015, 03:05:52 AM
I did see that a few companies offer gooving tool inserts with round tips, wonder if they would be any good, definitely alot smaller the a 6mm round for getting in tight places..

Sent from my XT1080 using Tapatalk

That is what I have with the SECO MDT tool.
Hood
Title:
Post by: lcvette on August 26, 2015, 08:14:50 PM
Ah ha...  I was going crazy looking for a 3mm round insert like the 6mm.   Ok ordered up the 3mm grooving tool holder and insert...  Good times ahead!

I just finished drawing te 17 tool holders and inserts I have and put them in the technology database for Camworks and went through and set all of the parameters up for each tool and filled my imaginary turret with all of the tools and told it to only choose tools from my turret for auto tool selection...

NOW I see the benefit of having everything properly setup.  I literally just draw up a solid model in solidworks, tab over to Camworks and hit the extract machinable features button and voila...  It defines all the features into turning operations be it is, I'd, groove, cutoff etc... Then I hit generate operation plan and it spits out a new tree for roughing and finishing each of the operations and then I hit generate tool paths and it pumps out a completed cam program based on all of the criteria I entered for each tool.  Very easy now that it is set up.  I can see this being very helpful for making parts quick from design to chip making.

Now I'm going to go set all my new tool holders up and set the heights and the re watch your video and start entering tools into mach3 with offsets and a master tool.

I guess after that I will be setup and ready to turn whatever pretty quickly.

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on August 27, 2015, 04:43:49 PM
Sounds like a nice CAM.

I have done another video with using home switches as the master tool position but its a bit scrappy and I am having issues trying to edit it. If I can't manage to get it sorted I will try and do another in the next day or two.

Hood
Title: Re: Gcode Request for a part
Post by: Hood on August 27, 2015, 06:12:15 PM
Here is the video, basically the same as before except I am using home switches as the master tool.
It is a bit shaky but hopefully still watch-able.
https://www.youtube.com/watch?v=Kla1sZ8IF6k&feature=em-upload_owner

Hood
Title:
Post by: lcvette on August 27, 2015, 11:10:15 PM
Nice!  I don't have home or limit switches that would work with the mill setup as a lathe so I will just have to use the master tool technique.  I think I am going to make a probe tool with a ball end to do the touch off on a 1" round gauge bar I bought  to zero in my mill probe tool.  I will put the round gauge in a piece of delrin and send some wires to the BOB and use it the same as you would a touch  plate for the mill.

The probe tool will be isolated by delrin as well for when I need to touch off on a part.  That should get all the tools dialed in to the master and the master dialed in to the work.

I was setting all my tool heights today by facing of some aluminum stock and trying to get the feel for where the right height was, I found the best height for surface finish was about .001"-.003" below the center point. Is that normal?  It doesn't leave hardly anything but a pin tip nipple that is barely noticeable.  Is this OK you think?

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on August 28, 2015, 02:54:57 AM
The right height for a lathe tool would be exactly on centre.
Parting tools may need very slightly above centre depending on the flex in tool/lathe. Boring bars may also benefit from being fractionally above centre depending on rigidity of bar and lathe.
I personally would never set below centre although a thou or so  would likely not make too much difference.

Hood
Title:
Post by: lcvette on August 28, 2015, 03:04:13 AM
Good to know,  I will give it another go in the morning... It may also be that the inserts I'm using weren't made for aluminum.  I noticed that the aluminum inserts have a bigger rake on the tips, perhaps that makes for a cleaner cut.  I have some inserts on the way for aluminum so perhaps I will be able to get the finish with it set dead on the center.  Thanks Hood!  And Im digging the videos! Very helpful!  Perhaps once I get everything dialed in I will get some video to share!

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on August 28, 2015, 05:25:10 PM
Yes, inserts specific for Alu usually have a high positive rake and are also usually ground and polished to give a sharp edge.
Having said that I usually don't bother with special inserts when doing Alu, but the results depend on the type of Alu being cut. Cast alu usually cuts nicely and as I do mainly marine work the alu grades I use cut fairly nice.
 I do not really like cutting Alu on the manual lathe, much prefer stainless :)

Hood
Title:
Post by: lcvette on August 28, 2015, 07:43:15 PM
Stainless?   I tried that on my mill and didn't get hang of it, tried allow, fast, deep cuts to avoid work hardening... Just ended up destroying endmills... Guessing machine rigidity had alot to do with it along with motor power.




Sent from my XT1080 using Tapatalk
Title:
Post by: lcvette on August 28, 2015, 08:23:17 PM
I think I know the answer to the question but I'm not positive and thought it best to ask.  When setting up the offset for a boring bar on the QCT post, do I set it off the back of the work piece?  Or should I use a piece of metal against the the stock and set it against the overhang of the metal off the edge of the stock?  I'm using mach standard mill with master tool mode and got a little confused in this part during the tool offset setup.

Thanks!

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on August 29, 2015, 03:54:01 AM
Stainless turns easily, just dont have the RPM too high and keep the feedrate up, it is similar for milling.

Setting boring bars up you can do it several ways.
You can take a cut of an internal diameter and measure.
You can, if you have enough travel, touch off the opposite side and enter a negative value.
You can use a piece of tool steel, or similar, held against the part and bring the tool out on X, you will easily feel as it touches.



Pic below of the last method although it is for the opposite hand of tool than I think you are using so is on the opposite side.
Title:
Post by: lcvette on August 29, 2015, 12:45:25 PM
That appears to be the same tool as the one I have.  I have enough travel to touch off the back no problem, so I will give that a try. 

Sent from my XT1080 using Tapatalk
Title:
Post by: lcvette on August 31, 2015, 05:53:18 PM
Hood,

I'm confused again..lol

I was reading the mach manual and it suggested letting the cam software handle the tool offsets?  Is that correct?

This is easy I'm sure, but I am terrified to crash this thing.  Do you let mach handle the offsets or your cam package?

Thanks!

Chris

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: lcvette on August 31, 2015, 06:56:02 PM
Ok,  I am glad i got confused because it forced me too look a little deeper and even with my cam package set for CNC Compensation off, it is still accounting for the tool tip radius.  I am using tools with a 1/64 (.015625") radius tip and it is showing the X going to X -0.156 on facing operations.. glad i caught that or it would have been doubled by mach if i entered the tool radius into the tool table.  so I know I can go back in and fix all of the tools I drew for Camworks and set the tool tip radius as a zero point and it will spit out unadulterated code and then have mach handle it, but it seems to me that letting the cam do it may be better?  keeps mach from having to do the calculations?  however, i need to now figure out what else this is going to effect such as part zeroing etc.  it appear there is a gauge offset in the camworks tooling table for both the X and Z in the tooling page.  it wants to set the offsets off of the flat of the square bar portion of the tool holder (the clamped section) for the Z and for the X it wants to offset from the rear edge of the tool.  when i zero them out it shows the offset to be the tool tip radius center point.  I wonder if I need to set the offset so the point shows the tool tip where it would be if there was no radius and the tip came to a point?  thoughts?

Soo confusing!
Title: Re: Gcode Request for a part
Post by: Hood on September 01, 2015, 05:52:55 PM
I don't know what your CAM calls the compensation but usually you have two types in the CAM.
In BobCAD they call it System Comp and Machine Comp.

System Comp will take into account the nose rad and you can also have collision detection so that it will take into account the shape of the insert (and holder if defined)
I have this turned on.

There is also machine comp where BobCAD will use G41 and G42 outputs  rather than producing a "true" toolpath code.
I have this turned off.

So basically I let the CAM handle the nose rad and collision detection and output the true path.
Mach itself handles the tool X and Z offsets.

Screenshots below showing the various options in BobCAD.

Hood
Title: Re: Gcode Request for a part
Post by: Hood on September 01, 2015, 05:53:59 PM
And this is the option I use, although occasionally I will use the option of no collision detection (last pic in previous post)

Hood
Title:
Post by: lcvette on September 01, 2015, 11:59:22 PM
Hood,

Excellent, that is exactly how I decided to set Camworks up as well.  It handles tool paths based on the tool models I designed and the zero point being the center of the tool tip nose radius so it is outputting true tool paths and I do the the X and Z offsets in mach3.  I have a part chucked up and am just tweaking the tool paths bit plan on hitting the go button tomorrow. 

I had been wrestling with the post trying to change the feed option between ipm and fpr and was stumped because the post template I was using, (fanuc generic) called for g98 or g99. finally out of the blue I saw a small check box on the fanuc source code in the universal post generator that asked if I wanted post style A, B, or C. Apparently B and C output that command as G94 and G95 which was what mach needs...  So now I'm in business and think the post is 100% mach compatible at least for anything I have test posted so far..lol

So thanks so much hood for the confirmation!  It also allowed me to run the same safety line up top without tripping error codes!

Double bonus!

Chris

Sent from my XT1080 using Tapatalk
Title:
Post by: lcvette on September 02, 2015, 09:03:48 PM
Ok, ran my first part, came out great but I ran into some issues with parting it off. stalled the motor with a horrendous shudder shortly after starting to cut.  I ended up manually parting it off running at 500 rpm and bumping in .001" at a time.

I was using 1000rpm and .0005" fpr...  What is a good rpm and feedrate for a parting tool?  It seemed to like 500rpm, but I'd like to get some experienced input.  I'm ready to start running parts now that everything is finally up and running, just need to dial in the part off.

Thanks Hood!

Chris
Title: Gcode Request for a part
Post by: lcvette on September 02, 2015, 09:07:44 PM
Oh and here is a picture of the finished test part.

(http://images.tapatalk-cdn.com/15/09/02/b6b991a70f5a2e88c304f3c1fd99c5a4.jpg)


(http://images.tapatalk-cdn.com/15/09/02/1d8689f38f01c381f528014055c85c1c.jpg)

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on September 03, 2015, 02:14:17 PM
Looking good :) Wee bit of chatter on the internal at the start but probably nothing to worry about.

Now parting, it will depend on material and the rigidity and power of the machine.
For me I usually just tend to stick to about 600 rpm and 0.1mm fpr(so that would be about 0.004" ) in stainless but depends on dia as well. Sadly Mach does not do CSS properly so you have to choose a rpm and go for it.

You insert manufacturer may have some info on surface speed and feed per rev but as said that may not be possible on your lathe depending on power of spindle and rigidity of the machine.

Hood
Title:
Post by: lcvette on September 04, 2015, 01:50:16 AM
Yeah I doubt it is rigid enough, it is actually not a lathe but my grizzly G0704 mill setup like a lathe with the head tilted sideways and a custom QTC tool post mounted on the end of the table and a R8  4" 3 jaw chuck. 

I will be running more parts tomorrow z a bit more complex, I will play with the feedrate for grooving and parting and report back with what I get to work...  I think I found part of the problem, the cutoff operation had an option for adding a chamfer and I Think the angle was a bit too aggressive.  I managed to do a successful groove today, it made a little bit of noise but then smoothed out and a nice stream of little square chips started flying out.  It then did great to widen the groove by using a 50% step over to wide the groove.

It did very well side cutting up to about 3/4 the length of the widened cutting tip, very smooth and very good surface finish.

Think I will just need to play with it and find out what the machine and cutter are happy with.  For now I will avoid the chamfer until after its made an initial groove instead of trying to cut into the stock by making a chamfer move... Think that's a bit too much for this machine.

Thanks again Hood!

Chris

Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on September 04, 2015, 03:21:03 AM
Not sure how you are doing the OD and ID but if doing the OD first then the ID it might be an idea to try it round the other way, it might get rid of the chatter on the ID. Then again it may give you some on the OD, just have to experiment.

Hood
Title:
Post by: lcvette on September 04, 2015, 12:19:14 PM
I bored first because I was afraid the small remaining material inboard would become problematic.  It would have only been about 0.11"  wall thickness supporting the part.  So as you suggested, I did my internal operations first.

I was using the boring bar that I crashed with, had an oops.. I checked everything on my design computer with a copy of machturn and it was fine but on my machine computer I had missed checking the box in the ports and pins config to reverse arc movements...  So it tried to make a loop into the interior part wall the first I, K move it got too... I found the tooling insert was chipped on the outer most edge near the back of the angle of the corner radius.  So the front radius was fine making a nice cut on the reducing slant wall where it was contacting the unchipped portion but on the straight in wall it was cutting partially on the chipped edge which probably didn't help... So new insert is now installed... Live and learn..lol



Sent from my XT1080 using Tapatalk
Title: Re: Gcode Request for a part
Post by: Hood on September 08, 2015, 01:53:08 PM
You will have many more "oops" moments on a lathe. People think they are much easier than a mill due to only having two axes rather than the three on a mill.
On a mill most of the time raising the Z will allow you to move X and Y safely, on a lathe you will find one  axes that needs to be moved before the other to make , sometimes the X will need moved before Z, sometimes the other way.

Hood
Title:
Post by: lcvette on September 10, 2015, 10:08:46 AM
Yes...  I see many easy ways to oops..lol.

I agree that the lathe could be significantly more dangerous, especially being the spindle is a large spinning mass verse an endmill.  I ALWAYS get nervous when the tool starts getting close to the chuck.. I watch the sims and know it will stop, but it is still a bit of a pucker factor no matter how many times I see it safely clear..hahaha

I did notice that grooving works great with a zig zag option I found in Camworks especially if it's a wide groove. It goes in a set depth then moves axially to the other edge and goes in the set depth again and back the other way and continues to the part geometry depth in X.  Definitely helps with the chatter.

I did find that 600rpm is perfect speed for grooving and parting off, excellent advice Hood!  I set feed for .001 FPR and it still chatters a little but but not nearly as bad.

I also found that parting off close to the chuck really makes a big difference. Almost eliminates all chatter and I was running .004 FPR with a nice smooth material peel.  I think it is because of several factors on my machine, for one the table mounted tool post is closest to the base so there is less deflection of the table and the material is closest to its mounting point.

All in all I call it a success..  Now I'm just digging deeper into the CAM software to find all of its nifty secrets, and there are quite a few.

The technology database has taken some time to figure out but now that I see how it works it is very powerful, and I love that it is completely configurable.  So for example, for ID Profiles, it has cored or solid parameters and for every various diameter o the ID profile it allows a configuration to be defined.  So for a 1" ID hole, I can program the auto feature recognition to call strategy #********* which has a center drill strategy with tool X, a drill strategy with tool Y, a bore rough strategy with tool Z, and a Bore Finish strategy with tool A. All of which pull from cutting parameters for each of those strategies.  Once you define those strategies for your machine but automatically recognizes the ID feature, generates an operation plan with all of the above strategies and then kicks out a tool path.  So it completely builds the machining plan and if all your setting are properly entered, it is done and ready to spit out a post.

Obviously setting all of the configurations takes time. But the tech database does have a wonderful copy function that allows you to copy a finished strategy parameter and paste it to another operation so it isn't too bad.  But for now I find it is easiest to set them up as I get to parts with features i haven't had before.



Sent from my XT1080 using Tapatalk