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

Oh and here is a picture of the finished test part.






Sent from my XT1080 using Tapatalk

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

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

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

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

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

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