1. Mathematical Quirk?

I was programming a cut with a ball endmill on a core of a mold I am building and I was getting an error on my cnc machine that said "Z NOT ALLOWED IN G17". Basically BobCad was putting a Z number in the program while doing a G02 or G03. I checked to make sure that my setup was to only put in Changed Z numbers and that was correct. I noticed this happened a couple of times before and I thought that it was because of my computer but then I was able to recreate the problem. It turns out that it has to do with the depth settings and I guess the mathematics involved in calculating the steps.

In the below example, the Z value is only placed in the G02 and G03 in every other step, which lead me to believe that it had to do with the math. I figured out how to avoid it, I just adjust the steps or the depth settings, but it was a real pain in the rear to figure out, I thought I'd help someone else out by telling you guys about it.

Here is an example of the code:
G00X-10.Y8.Z0.05
X-8.5851Y-0.9766
G01X-8.5851Y-0.9766Z-0.2083F3.0
G03X-8.3176Y-1.2441I-8.3176J-0.9766K-0.2083F10.0
G01X-4.6936Y-1.2441
G02X-4.1365Y-1.3724I-4.6936J-2.5175
G01X-3.6812Y-1.5939
G03X-3.1369Y-1.7193Z-0.2082I-3.1369J-0.4752
G01X3.1369Y-1.7193Z-0.2083
G03X3.6812Y-1.5939Z-0.2082I3.1369J-0.4752
G01X4.1365Y-1.3724Z-0.2083
G02X4.6936Y-1.2441I4.6936J-2.5175
G01X8.3176Y-1.2441
G03X8.5851Y-0.9766I8.3176J-0.9766
G01X8.5851Y0.4731
G03X8.3176Y0.7406I8.3176J0.4731
G01X5.0814Y0.7406
G02X4.5074Y0.9974Z-0.2082I5.0814J1.5105
G03X3.9552Y1.2445Z-0.2083I3.9552J0.5039
G01X-3.9552Y1.2445
G03X-4.5074Y0.9974I-3.9552J0.5039
G02X-5.0814Y0.7406Z-0.2082I-5.0814J1.5105
G01X-8.3176Y0.7406Z-0.2083
G03X-8.5851Y0.4731Z-0.2082I-8.3176J0.4731
G01X-8.5851Y-0.9766Z-0.2083
X-8.5851Y-0.9766Z-0.2165F3.0
G03X-8.3176Y-1.2441I-8.3176J-0.9766K-0.2165F10.0
G01X-4.6936Y-1.2441
G02X-4.1365Y-1.3724I-4.6936J-2.5175
G01X-3.6812Y-1.5939
G03X-3.1369Y-1.7193I-3.1369J-0.4752
G01X3.1369Y-1.7193
G03X3.6812Y-1.5939I3.1369J-0.4752
G01X4.1365Y-1.3724
G02X4.6936Y-1.2441I4.6936J-2.5175
G01X8.3176Y-1.2441
G03X8.5851Y-0.9766I8.3176J-0.9766
G01X8.5851Y0.4731
G03X8.3176Y0.7406I8.3176J0.4731
G01X5.0814Y0.7406
G02X4.5074Y0.9974I5.0814J1.5105
G03X3.9552Y1.2445I3.9552J0.5039
G01X-3.9552Y1.2445
G03X-4.5074Y0.9974I-3.9552J0.5039
G02X-5.0814Y0.7406I-5.0814J1.5105
G01X-8.3176Y0.7406
G03X-8.5851Y0.4731I-8.3176J0.4731
G01X-8.5851Y-0.9766
X-8.5851Y-0.9766Z-0.2248F3.0
G03X-8.3176Y-1.2441I-8.3176J-0.9766K-0.2248F10.0
G01X-4.6936Y-1.2441
G02X-4.1365Y-1.3724I-4.6936J-2.5175
G01X-3.6812Y-1.5939
G03X-3.1369Y-1.7193Z-0.2247I-3.1369J-0.4752
G01X3.1369Y-1.7193Z-0.2248
G03X3.6812Y-1.5939Z-0.2247I3.1369J-0.4752
G01X4.1365Y-1.3724Z-0.2248
G02X4.6936Y-1.2441I4.6936J-2.5175
G01X8.3176Y-1.2441
G03X8.5851Y-0.9766I8.3176J-0.9766
G01X8.5851Y0.4731
G03X8.3176Y0.7406I8.3176J0.4731
G01X5.0814Y0.7406
G02X4.5074Y0.9974Z-0.2247I5.0814J1.5105
G03X3.9552Y1.2445Z-0.2248I3.9552J0.5039
G01X-3.9552Y1.2445
G03X-4.5074Y0.9974I-3.9552J0.5039
G02X-5.0814Y0.7406Z-0.2247I-5.0814J1.5105
G01X-8.3176Y0.7406Z-0.2248
G03X-8.5851Y0.4731Z-0.2247I-8.3176J0.4731
G01X-8.5851Y-0.9766Z-0.2248
X-8.5851Y-0.9766Z-0.233F3.0
G03X-8.3176Y-1.2441I-8.3176J-0.9766K-0.233F10.0
G01X-4.6936Y-1.2441
G02X-4.1365Y-1.3724I-4.6936J-2.5175
G01X-3.6812Y-1.5939
G03X-3.1369Y-1.7193I-3.1369J-0.4752
G01X3.1369Y-1.7193
G03X3.6812Y-1.5939I3.1369J-0.4752
G01X4.1365Y-1.3724
G02X4.6936Y-1.2441I4.6936J-2.5175
G01X8.3176Y-1.2441
G03X8.5851Y-0.9766I8.3176J-0.9766
G01X8.5851Y0.4731
G03X8.3176Y0.7406I8.3176J0.4731
G01X5.0814Y0.7406
G02X4.5074Y0.9974I5.0814J1.5105
G03X3.9552Y1.2445I3.9552J0.5039
G01X-3.9552Y1.2445
G03X-4.5074Y0.9974I-3.9552J0.5039
G02X-5.0814Y0.7406I-5.0814J1.5105
G01X-8.3176Y0.7406
G03X-8.5851Y0.4731I-8.3176J0.4731
G01X-8.5851Y-0.9766
G00X-8.5851Y-0.9766Z0.05

2. Jim,
You'll have to go into your nc editor in Bobcad, and open up the setup, and then conversion. This will be where you enter a generic version of what Bobcad posts in the left hand window, and then the conversion should be put in the right window.

The conversion amounts to simply dropping the Z and K words from the G02/G03

There are special codes that you use and I think it tells you somewhat about this in the help file. For example, to remove all instances of K, you would use this in the "Original" window:
K-*[0-9]*.[0-9]*
And on the same line directly across from this in the "Convert to" window, you simply leave a blank.

The basic idea is that you will likely never have need to use a Z nor a K value in your G02/G03 lines, so you remove them in this fashion.

3. The Z can be a problem, but if you use this conversion you will never see it again.

In the Original Window put in this value
{G03}@ {[A-Z]*-*+*[0-9]*.[0-9]*}@ {[A-Z]*-*+*[0-9]*.[0-9]*}@ {[A-Z]*-*+*[0-9]*.[0-9]*}@ {[A-Z]*-*+*[0-9]*.[0-9]*}@ {[A-Z]*-*+*[0-9]*.[0-9]*}@ {[A-Z]*-*+*[0-9]*.[0-9]*}@

Red will be the X value, Yellow the Y value, Magenta the Z value, Blue will be the I value, Lime the J value and light blue the K value.

In the Convert to window put in this string
@1@ @2@ @3@ @5@ @6@

This would remove both the Z and the K value. You would have to enter the command in with G02 as well.

In fact you could possibly correct any problems that might come up in the future using this conversion method in your post processor.

Regards

4. Thanks for the replies. I tried inputing the conversion, but I must have not gotten it exactly right, however, I did use the REPLACE function to strip all the K values from my programs. I'll give this some more thought tomorrow and triy some other things out. One thing I don't understand is when you refer to the post processor, can this be edited without using the SETUP function? I edited a post processor for Mastercam a couple of years ago (changed it from using I &J to using R values), but I wasn't aware that I could edit the post processor for BobCad. Where would I go to get more info about doing that?
Jim

Posting Permissions

We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!