Results 1 to 20 of 24
06-12-2013, 01:28 PM #1
Programming with tool nose radius.
Who here programs with tool nose radius? If I program with tool nose radius, my program is created
with all my depths and everything deeper by half the tool nose radius. If I choose to program this way, I have to
tell the machine the tool nose in the machine?
By choosing to NOT program with the tool nose radius, basically, a point to point program, will I have any problems?
06-12-2013, 01:50 PM #2
unless your parts have no chamfers/angles/radii/etc. you'll need to figure for the nose radius.
06-12-2013, 02:10 PM #3
Now if I program for tool nose radius, do I have to enter a raidus in the machine under the tool nose comp?
06-12-2013, 02:28 PM #4
Depends, are you using a program to generate the code or manually coding it at the machine?
06-12-2013, 03:06 PM #5
06-12-2013, 03:25 PM #6
if you can post the code to the contour. I've had similar happen when I used the the wrong cutter comp on the sub-spindle.
But the cam systems I've seen you can have it do the tnr for you and the coded will be changed from the print.
Personally I would never do it that way. I perfer to have all code to the print and use the control to comp and do the math.
EnderDRM liked this post
06-12-2013, 03:54 PM #7
I define my TNR in my cad. It compensates for the chain I select to cut, whether it be mill or lathe. I let Mastercam decide the code. Programming center of the cutter on a mill is old school compensation. Didn't even know people still did that, lol.
06-12-2013, 03:58 PM #8
What line of code is the G40 on? I have had similar issues depending on what line the comp. cancel is on. work around was duplicating the move once off the part,
G1 X 2.5
G1 X 2.5 G40
Also are you using a canned cycle or long hand?
06-12-2013, 04:14 PM #9
My only experience, 23+ years, with CADCAM is Edgecam and its predecessor Pathtrace. It has a facility called "Pathcomp" in which all the TNR comp is handled to whatever TNR you tell it to use. On the first lathes I programmed, I set the R value to zero for all tools on the machine. Never had a problem with unexpected cuts or "no cuts".
On the POS Anilam control I do not use "Pathcomp" with the canned cycles. It wants to do a TNR comp(of unpredictable amounts) even if the R value is set to zero in the table. Set the R value to what tool I'm going to use and most of the time the result is acceptable. If I'm not using a canned cycle, "Pathcomp" handles comp correctly because the machine isn't using a G41/G42.
Fanuc controls I program without 'Pathcomp" because the control works okay.
Fagor controls I mostly use the conversational stuff.
06-12-2013, 04:45 PM #10
On the Anilam 4100T control I run its very important to have the proper "L-Code" set in the offsets/tnr/wear window. The L-Codes tell the control how the tool is positioned in relation to the workpiece (Boring bar has a L-Code separate from a turntool). The result if the L-Code was wrong would be the diameter of the part would end up 2X the tnr big or small depending on your compensation(g41/42).
06-12-2013, 05:08 PM #11
06-12-2013, 07:06 PM #12
Are you programming to the tip of the radius or to the center of the radius?
06-13-2013, 05:34 PM #13
Here is my sample code that is confusing me.
G1 Z-2.6472 F.015
G0 X3.648 Z-2.6382
I am wanting to turn the diameter in Z to 2.6"... I don't see what the tool nose radius has to do with making the machine cut deeper. PLEASE EXPLAIN!!
I understand why the tool has to go further in X to face the part but further in Z? I touch off on the lead edge as shown in the pictures.
Image - TinyPic - Free Image Hosting, Photo Sharing & Video Hosting
06-13-2013, 05:48 PM #14
If you're touching off the leading edge of the tool, and you want the leading edge of the tool to be 2.6 deep, then you program it to Z-2.6.
How did you end up with the Z-2.6472?
06-13-2013, 06:01 PM #15
06-13-2013, 06:11 PM #16
06-13-2013, 06:26 PM #17
06-13-2013, 06:28 PM #18
Lets say you're programming a 1" diameter turn, that goes 1.5" back, then goes to 2" diameter with a .015 radius on the corner. Tool in the machine has a .032 radius tip on it.
Without cutter comp. the program should look like this:
G00 X1.00 Z.1
G03 X2. Z-1.542 R.042
G1 blah blah blah
Now with cutter comp:
G00 X1.0 Z.1
G1 G42 Z0
G03 X2. Z-1.51 R.01
G1 blah blah blah
The only thing cutter comp. really effects is how you program your radius or chamfers on shoulders or corners. The O.D. and I.D. diameters and depths are programmed the same either way.
Now, if you're programming on cad/cam, and you're getting numbers that are compensating for the radius of the tool you're using on your depths and diameters, that sounds like a setting that needs to be changed in how the cad/cam uses cutter comp. Perhaps you might be better off asking your question in the cad forum? I'm not real fluent on those systems, or maybe you have an odd control at the machine?
06-13-2013, 07:45 PM #19
06-18-2013, 02:59 PM #20
I would be very interested in knowing what machine your programing, control and with what software. I either wright the program by hand exactly like Dave K said using the G42 and put the tool nose radius and tool type in the offset page. Or when I use Virtual Gibbs I tell Gibbs that information and get something like the following. I have had machines that if I put it in would automatically comp for the Rad if put in the offset page so since I have already compensated with the software and no need for it I don't put that information in the offset page the software has already done the compensation.