Problems with Pawn Program <solved>

[Norton]

Hello, I just completed converting a Grizzly G0765 lathe to cnc using a Centroid Acorn and a Gecko G540. I have set the X and Z axis Tool Offsets for an OD Tool by following the instructions in the Centroid manual and watching Franco's great video. In fact, I have done this many, many times over the past 4 or 5 days. Each time I try to run the Pawn program after homing the lathe it initially appears to go to the correct X and Z locations. Then it immediately starts the X axis in the + direction and continues until it trips the limit switch.

I followed cnc_Keith's video on Conversational Programming and it will run this without issue. I realize this program is not as complex as the Pawn program.

Please find attached a Report. I hope I did it correctly.

If someone could please help me with this I would greatly appreciate it.

Thanks,

Norton

[cncsnw]

What does it look like when you preview it on the F8/Graph screen?

[Norton]

Thanks for your help. I will try to upload a screen shot of it first thing tomorrow.

[Norton]

Please find attached a screen shot of the PAWN graphic view. Doesn't look right to me but then again what do I know? LOL

Thanks again for your help

[cncsnw]

If you are going to run a program which calls for tools 7 and 8 (for example), then you need to measure or set correct (or, for a dry run, at least workable) X and Z offsets for those tools.

If you look at your report, you will see that:
1) Your part zero location (WCS #1 offset from machine home) is about Z+2.2, X+0.86 (radius)
2) Your tool #2 offsets are about X-3.3 (radius), Z-12.7
3) Your tool #7 and #8 offsets are all zero

The copy of the pawn sample program that I have uses T7 and T8. Your copy may be different.

The first move in the pawn program is to bring X to a clearance diameter of X0.85, and Z to a clearance of Z+0.1.
If you were using T2, then going to that location would mean moving X to a radius value of 0.86 + 0.425 - 3.3 = X-2.015 from X home.
If you are using T8, then going to that location requires moving X to a radius value of 0.86 + 0.425 + 0.0 = X+1.285 from X home.

So it is likely that the problem is you are using tools with incorrect offset values.

Some general advice for troubleshooting this type of problem:
- Measure and set your software travel limits, so the control can tell you about the problem before it even begins the move.
- Run the program in single-block mode
- While running the program, watch the DRO position (what X and Z does the control think the tool tip is at?)
and watch the tool number display in the status window (what tool offset number is active?)

[Norton]

I am going to read and continue to reread what you posted until it all registers in my head. I did a new tool offset for Tool 02 as this is the only OD tool I am using at this moment. I want to get this working correctly then I will do all my tools. This is the steps and procedure I followed to set Tool 2:

1. Home machine
2. Made sure Tool 02 was active
3. Took skim cut from stock
4. Measured diameter = 0.4860
5. Opened Tool Geometry Offset Library F1-Setup > F-2 Tool Offset
6. Moved cursor to X offset column in Offset Library
7. Pressed F1-X Diam
8 Entered 0.4860 in the "Establish the X Diameter field"
9. Then pressed F10-Save
10. Press F-2 Measure Tool
11. Press F5 Measure Offset X

Setting for WCS #1 (G54)

12. Pressed space bar to select yes to save to all WCS
13. Pressed F8-set X

Ran the Pawn program and it did the same thing. As a test I issued a G0X0 in MDI and it brought the tip of the tool to the exact X0 position.

Anyway, thanks so much for your help. Please let me know if you see any problem in my steps.

[Norton]

Also, I noticed that Tool 01 is gone from the Tool Library. I don't know it this means anything but thought I would let you know. If you check me procedure and it looks OK, what do you think about removing and reinstalling the software?

[cncsnw]

Regarding tool 1: did you try using the up arrow key?

Regarding the pawn program: do you know which tools are called out in the program? If you are not sure, post a copy of the program you are trying to run.

[Gary Campbell]

Like you when I first attempted to run the pawn program my only setup OD tool was T#1.

I edited the file to use T1 and aborted out of the file when the toolchange to the parting tool was called.

[Norton]

Thanks cncsnw, that solved the mystery of the missing T01.