Tool Control Tolerances for Routing a Hole

CNC pros try to figure out why a CNC router is making lockset holes out of round. The culprit may be a problem with tool compensation in the lead-in and lead-out routine. September 24, 2006

We are having problems cutting an extrapolated pocket (lock hole) on our Rover 20. All the geometry is accurate, but when it comes to that hole (which we cut with the router, since all our spindles are used), it is constantly out of whack. We are relatively new with that machine and I suspect that speed is an issue. We use a 1/2" bit to cut a 5/8" hole, and dropped the speed to 100 entry, 500 cut from the standard 1000 / 5000. The hole is at least 1.5 mm out. We do the same thing on our router and have no problem (retrofitted Thermwood C50). Any thoughts?

Forum Responses
(CNC Forum)
From contributor S:
Are you using one of the macros that came with controller to route the hole?

From the original questioner:
No, I just run a tool path inside the hole perimeter, and drop feed, as well as program 19 mm cut in 2 passes.

From contributor S:
I doubt if speed is the issue. The obvious test for that is to set the speed at low level. I don’t know what kind of lead-in you are using, but one thing I would try is to route the hole with a tool that is smaller than the radius of the hole. For example, try a ¼” tool just to rule out any lead-in issues. If you post your code here, that might help us to see if it is a programming issue.

From contributor W:
I run a Rover 24 and here is the code I use for a 5/8" hole in a 1.80" thick door. Just enter the X origin # and the Y origin # to position the hole.

N30 PAN=1 ST1="EM1/2" ST2="NULL" ST3="NULL" L=PCUA
N39 XO=0 YO=0 G0
N40 G46 X0.003*25.4 Y0.000*25.4 TP1 PRF=0.905*25.4 F=4.0 G42 VF=3.0 L=PON M55 AX=X,Y,Z
N50 X0.323*25.4 Y0.000*25.4 G1
N60 X-0.323*25.4 Y0.000*25.4 R0.323*25.4 G4
N70 X0.323*25.4 Y0.000*25.4 R0.323*25.4 G4
N80 G40 X0.003*25.4 Y0.000*25.4 G1
N100 G46 X0.003*25.4 Y0.000*25.4 TP1 PRF=1.810*25.4 F=4.0 G42 VF=3.0 L=PON M55 AX=X,Y,Z
N110 X0.323*25.4 Y0.000*25.4 G1
N120 X-0.323*25.4 Y0.000*25.4 R0.323*25.4 G4
N130 X0.323*25.4 Y0.000*25.4 R0.323*25.4 G4
N140 G40 X0.003*25.4 Y0.000*25.4 G1

From contributor T:
If you are using offline software, it may be a post processor issue. If this is the case, you can test it by creating the same circle in the control software and comparing the results.

From the original questioner:
Thanks for all the input.
- I do not use any lead in/out at all, on this cut.
- We post process directly at the controller (NC 410).
- We go directly from a DXF R12 file layered according to Biesse; this particular cut is in the layer Router19.
- We program the tool path as follows:
Cut direction CW
Compensation : DX (right of line)
Number of cuts 2
Entry speed : 100
Feed speed : 500

The result is a hole oversized by about 1.5 mm, slightly out of round. That's why I was questioning feed and speed. Thanks for the code. Unfortunately, even though I program all our router G code without a hitch, I still have to figure out Biesse weird code as well as a way to write it and input it off line. This is why we strictly import dxf to the controller and post process at the machine.

Someone emailed questioning compensation, but since we use a 1/2" cutter, if it was a comp error, the hole radius would end up being 1/4" too big, which is not the case. By the way, anyone familiar with the NC 410 and practical ways to program it off line aside from using the NC 410 software and network…? We do have a very good cad cam package, but were not able to supply our developer with any code examples that made any sense.

From contributor G:
In using a 1/2" cutter to create a 5/8" diameter hole, I would definitely question the feed speed. Plunge at 50 IPM and continue your path at 50 IPM. Make 2 complete passes around the hole. In this case, your cutter is barely moving, so the slow speed is not really that slow. I don't think you will have heat issues, but watch it carefully and use a bit of air to blow out the chip. Also try cutting this CCW, as it is an inside hole. You may be getting some deflection from the back side of the cutter with a clockwise cut. That's a big maybe.

From contributor G:
Duh. Cutting clockwise *is* the way to go. Forget what I mentioned about cut direction above.

From contributor J:
Is the entire hole oversize by ~1.5mm, or is it out of round?

From contributor W:
Since you said you were using compensation, remember that you need half the diameter of the tool for a lead in and lead out for it to work. This can be very tricky to have a .25" lead-in with a 1/2" tool inside of a 5/8" finished hole size. I know in Mastercam it took me a while to get the arc right so the tool would not hit the outside radius of the 5/8" hole. I would try a hole without comp, plunge in the middle of the circle, move over 1/16", then do the arc and see how that works.

From contributor W:
Or simply turn the compensation ( DX ) off and run a test piece.

From the original questioner:
I use no lead at all, only comp. I think it's speed more than anything, and not used to program speed in metric. On our router, I have to get down to about 15 IPM to cut the same hole without problems.

From contributor W:
I'm not sure if you realize this, but in order to use compensation, you are using a lead in and lead out, also known as linear and circular attach and detach in Biesse code, and I'll bet that is your problem.

From the original questioner:
No, I did not realize that. I assumed that by selecting NO for lead in lead out, the bit would just simply drop on targeted xy position, only compensating by half the cutter width. Did not know that compensation has a built-in lead... That's odd. On our other controller, I can choose comp, as well as no lead at all.

From contributor W:
When using comp, the bit needs to move at least half the diameter of the tool to move to either the right or left side of the shape to be cut. That is probably why your 5/8" hole is not round. Like I said in an earlier post, it took me a while to get it right in Mastercam. I'm not 100% sure if xnc and 410 codes are the same, but try to type in the code above and see if it works.

From the original questioner:

Thanks, I will.

From contributor J:
That's why I asked you if the hole was not round, because of tool comp issues. If you will read one of the first replies in this thread, he suggested that you try a 1/4" bit. I'll bet that's why.

There is a way to cut a 5/8" hole with a 1/2" bit. Start/end in the center of the hole (not tangent to the inside edge), use circular attach/detach with an incremental move XI or YI=radius for the hole. Also set the attach/detach R value equal to the hole radius. In that way, the tool will plunge in the center of the hole, swing out to the edge, cut the hole, then swing back in to the center of the hole. For such a small hole/large tool, you must be sure you have the tool diameter exactly right in the controller data.

From contributor M:
Manually move the machine head into the center of the work table (x Direction). Go behind the machine and physically push the tool head back and forth again in the "x" direction with the machine in manual mode. If you feel any movement whatsoever, the "x" rack and pinion drive are worn, thus the weird holes. If you had any kind of programming problem, your software would be giving you errors. How do I know? Been there, done that, and not real cheap to fix. When it's fixed, clean it and grease it regularly.