# First CNC'ed Part Made on My PM25 Mill



## devils4ever (Apr 7, 2020)

Very exciting times. I finished my CNC conversion of my PM25 mill and made my first part. Since the CNC conversion kit I bought didn't have a cover for the column where the handwheel was located, I decided to make one. It's a simple project, but I learned a lot. I used FreeCAD for CAD/CAM and LinuxCNC on the mill PC.

Heres' the 3D view of the part.




The biggest challenge was trying to determine how to hold this part since it's machined on all 4 sides. I came up with this for a solution.
1. Use a vise to hold the part and only do the drilling operation.
2. Clamp the part to the table with a 1-2-3 block underneath. Only clamp the 2 long sides in the middle. Set the Z distance so it clears everything. Use the quill to manually drop down to the part. As the tool nears the clamps, raise the quill. I single stepped the G-code for this.
3. After this is done, add clamps on the 2 short sides. Then, remove the clamps on the 2 long sides. This ensures the part doesn't move. Manually position the end mill and complete the uncut sections on the long sides.

Does anyone have suggestions on how to do this differently?

Take a look.




It turned out better than expected. As for dimension accuracy, I got about 0.002" undersize on the short dimension and about 0.003" oversize on the long dimension.


----------



## JimDawson (Apr 7, 2020)

devils4ever said:


> Does anyone have suggestions on how to do this differently?



Clamp a ''spoil board'', could be another piece stock in the vice or an actual MDF or particle board screwed to the table.
Drill & tap the screw holes in the spoil board
Clamp the part to the spoil board
Drill the screw holes
Install screws
Profile the outside.

See how I do it here https://www.hobby-machinist.com/threads/press-feeder.82699/#post-723662


----------



## devils4ever (Apr 7, 2020)

Got it! That's a good idea. I got part of it right by drilling the holes first, then doing the profiling.

I'm just happy to see rounded corners! I know it's not much, but I could never do that manually on the mill. I've had to cut and file to do that.

Great thread you sent. I won't feel so bad when I break an end mill when someone as seasoned as you do it. 

I still have to learn feed rates. I had the end mill taking 0.100" DOC at 5 IPM. For drilling, I had the feed rate set to 1 IPM. Both seem to work fine. I'm in no rush.


----------



## Mini Cooper S (Apr 7, 2020)

Congratulations, looks good.

Richard


----------



## bakrch (Apr 7, 2020)

Nice end mills are key for finding efficient feed/speeds. YG1 ALU-POWER is what I like to use.

Here is the 1/2" YG1 28593 end mill at work on a fairly stock PM25MV. I prefer the 3/8" 28584 but sometimes need the longer reach of the first end mill.

I have to conventional mill to avoid chatter (due to backlash), but you may not have to if you have decent ballscrews and nuts.


2500RPM .035 radial, .62 axial, .0069 IPT (51.7 IPM)

__
		http://instagr.am/p/B-NlUWpnCc3/


----------



## devils4ever (Apr 7, 2020)

Luckily, I don't seem to have a chatter/backlash issue. Climb cutting is way smoother than conventional cutting.


----------



## devils4ever (Apr 8, 2020)

I tried my second CNC project creating a round knob with circular cutouts. It ran great and looked really good. However, after measuring the lobes on the knob, I found that the knob is not exactly round. There are 6 lobes and measuring across the 3 pairs, I found two measured about 0.995" and the last one measured 0.988". That's a difference of 0.007". I'm assuming this is from backlash. Does this amount of backlash seem reasonable or excessive? I have double ball nuts for the purpose of reducing backlash. For this application, it doesn't hurt anything, but for other projects it could matter.


----------



## JimDawson (Apr 8, 2020)

devils4ever said:


> I tried my second CNC project creating a round knob with circular cutouts. It ran great and looked really good. However, after measuring the lobes on the knob, I found that the knob is not exactly round. There are 6 lobes and measuring across the 3 pairs, I found two measured about 0.995" and the last one measured 0.988". That's a difference of 0.007". I'm assuming this is from backlash. Does this amount of backlash seem reasonable or excessive? I have double ball nuts for the purpose of reducing backlash. For this application, it doesn't hurt anything, but for other projects it could matter.



Something is seriously wrong.  As far as backlash, with double nuts I would expect 0 backlash and would not accept more than that.  So first check the machine for backlash to see if that could be the problem.

Then cut a circle and see what you really have.  Motor tuning could be in play here also.  There are a number of things that can cause this, but check the mechanical first.


----------



## Shootymacshootface (Apr 8, 2020)

Although I personally ha e never done so,but I know that super glue or two sided tape is often used for hard to hold parts. Congrats on the new machine!


----------



## devils4ever (Apr 9, 2020)

JimDawson said:


> Something is seriously wrong.  As far as backlash, with double nuts I would expect 0 backlash and would not accept more than that.  So first check the machine for backlash to see if that could be the problem.
> 
> Then cut a circle and see what you really have.  Motor tuning could be in play here also.  There are a number of things that can cause this, but check the mechanical first.



I placed my Last Word indicator in on the spindle and jogged the X-axis back and forth by 0.010". The indicator moved about 0.009" showing about 0.001" of backlash.

Then, I tried the same for the Y-axis. It showed 0.005" of backlash. So, I think this is the cause. I tried tightening the mounting screws and the screws on the coupler, but it didn't seem to help. The Y-axis has a threaded end on the ball screw. So, I tried loosening the screw on the coupler and locking the table and advancing the table a few thousandths to see if that would tighten it. That didn't seem to have any affect. I'm assuming there's some play where those bearings are in the mount. Any other ideas?


----------



## bakrch (Apr 9, 2020)

It is most likely due to improperly set preload between the two ball nuts.  Not sure what software you are running, but you can likely compensate for it until you are able to fix.  I have about .002-.0025 on each axis, and even that is enough to give an undesirable performance.


----------



## devils4ever (Apr 9, 2020)

Yeah, I tried to tighten the coupler to the threaded section on the ball screw, but I think I might have made it worse.

I can push and pull along the Y-axis and get the table to move 0.005". How do I set the preload on the ball nuts?

I'm running LinuxCNC. Is there a way to compensate for it here?


----------



## bakrch (Apr 9, 2020)

devils4ever said:


> Yeah, I tried to tighten the coupler to the threaded section on the ball screw, but I think I might have made it worse.
> 
> I can push and pull along the Y-axis and get the table to move 0.005". How do I set the preload on the ball nuts?
> 
> I'm running LinuxCNC. Is there a way to compensate for it here?



There is a spacer in between the ball nuts that is likely undersize. You need to remove that and replace with a stack of belleville springs. To disassemble you will need to make a tool to keep the balls from falling out. Assuming you have 1605 size, I can hook you up with those dimensions if you need them.

Here is what my X-axis looks like: 



https://imgur.com/UOkA1gd


I have a ton of work right now though and haven't gotten around to fixing yet. 

Not sure about Linux CNC, but as popular as it is ... can't imagine that it doesn't have backlash comp.


----------



## devils4ever (Apr 9, 2020)

Yeah, that looks pretty tricky. A spacer has to go in between the ball nuts? You can't just spread them apart and re-tighten the screws?

I did find how to add backlash compensation to LinuxCNC. A quick test seems to confirm that it works.

I plan on milling a 3.000" circle soon, so I'll see how well it does.


----------



## bakrch (Apr 9, 2020)

devils4ever said:


> Yeah, that looks pretty tricky. *A spacer has to go in between the ball nuts?* *You can't just spread them apart and re-tighten the screws?*
> 
> I did find how to add backlash compensation to LinuxCNC. A quick test seems to confirm that it works.
> 
> I plan on milling a 3.000" circle soon, so I'll see how well it does.



There is already a spacer in there, but it was not sized with care. The spacer is a 2pc split bushing and the key goes from one ball nut, through the spacer groove and into the other ball nut (see my vid for reference). You could make your own spacer to replace if you have the means. Belleville springs are a much simpler solution and will force the ball nuts to remain apart (preload) without the task of making a precision part.  The only drawback is the trial and error to get the correct force to resolve the issue all without going too tight, which would prematurely wear on the system.


----------



## JimDawson (Apr 9, 2020)

The other place that backlash can come from is the ball screw end bearing.  That needs to be preloaded also.


----------



## devils4ever (Apr 9, 2020)

JimDawson said:


> The other place that backlash can come from is the ball screw end bearing.  That needs to be preloaded also.



I never heard of Belleville springs. I'll have to look into that.

I _think _I have the ball screw end bearing as tight as I can get it. I'm not 100% sure, but I loosened the set screw on the collar, locked the saddle, and snugged the collar against the bearing while tightening the set screw. I've done this 3 or 4 times now.

I'm guessing getting rid of the mechanical backlash is preferable to having the backlash compensated for in the LinuxCNC software?


----------



## JimDawson (Apr 9, 2020)

devils4ever said:


> I'm guessing getting rid of the mechanical backlash is preferable to having the backlash compensated for in the LinuxCNC software?



Much preferable, backlash comp in software is OK(ish), but there is no substitute for a mechanically tight machine.


----------



## shooter123456 (Apr 27, 2020)

devils4ever said:


> Does anyone have suggestions on how to do this differently?


My preferred method is using a set of low profile clamps (Something like Mitee Bite talon clamps) that hold on to a small bit of stock, machine the top side on all 4 sides + the face, then flip it and deck off the gripped portion.  It usually requires oversizing the initial stock somewhat, but it can be avoided if you are careful.



devils4ever said:


> I _think _I have the ball screw end bearing as tight as I can get it. I'm not 100% sure, but I loosened the set screw on the collar, locked the saddle, and snugged the collar against the bearing while tightening the set screw. I've done this 3 or 4 times now.


What kind of bearings are you using?  If they aren't set up to provide preload, it doesn't matter how much you tighten it, it won't get any better. That also isn't a great way to tighten the ballscrews into place since even with locked axes, the ballscrews may be able to move them.  I also found that the standard lock nuts aren't very good for locking the ballscrews and staying locked.  The set screw doesn't hold well and damages the threads.  

I made some lock nuts that do a much better job and are easier to tighten.


----------



## devils4ever (Apr 27, 2020)

I got the kit from Dave at ArizonaVideo, so I'm not 100% what bearings are used. You can see some pics here, but I'm not sure if you tell from these pics.

I might try the Belleville springs if I can determine the correct ones to use. I did add a backlash term to LinuxCNC, but I don't think it helped much. I'm still seeing a difference of about 0.007" and 0.008" in the diameter.


----------

