How to change prefix to finish_number_of_cuts variable?? (Mach3 posting BobCad V24)

[NICKKINSMAN]

Hello;

I've gotten my threading post very close to working well in the processor, but I cannot figure out how to change the prefix to the finish_number_of_cuts which brings in the spring passes. It defaults to "D" and I can't find the question anywhere in the postprocessor to change it. I looked though all the other post processors for Mach3 as well and could not find it. I assume there is probably a reference line somewhere that is not put in the file I have, as there are lots of skipped processor line blocks. Does anyone know where the reference guide is showing what each line number is referenced to, or specifics to this reference line?

Here is what I have in threading 87 processor line:

87. Start of thread (G76) cycle
n,"G76",thread_x2,thread_z2,thread_lead,thread_fir st_cut,thread_angle_in,thread_machine_allowance,th read_last_cut,finish_number_of_cuts,"L360 (Remove if no chamfer)"

Thanks.

Similar Threads:

• BobCad V23 Posting Issue?
• Bobcad V26 4th axis posting
• Need Help!- Bobcad V25 Not posting ???
• Need Help!- G41 Not posting (Bobcad V24)
• Need Help!- Mach3 or BOBCAD - Tool Change Halt Wanted

[SeanDa]

Nickkinsman,

After taking a look at the post processor, it does not appear we have an area in which this can be changed. What I went ahead and did was created a script to output the value with a letter designation that can be changed by you. To implement this into your post processor, the first thing that will need to be done is update the version at the top of the post to 10.0. Then you will past this code into program block one, which if it does not exist in your post processor, you will create a block number 2001. Then underneath this, you will past the script that is below. Then change the finish_number_of_cuts to program_block_1. You can change letter designation easily by changing the D in the parenthesis to whatever letter you want output.

Script:
Dim finishPass
finishPass = CALL Lathe_GetFinishNumberOfCuts()
Lathe_SetReturnString("D"&finishPass&"")

[NICKKINSMAN]

Wow, I am very surprised there is no variable for this, I would have thought every possible threading option would have a variable since they vary so much between machine controls, making it easy to set them up. No matter though - thank you for the reply. I will give this a try next week, I am away from my work computer over the weekend. I'll report back if it works!

Thanks again.
Nick

[NICKKINSMAN]

Sean;

I gave it a run, but I am getting a syntax error on the program block line - attached is a screenshot of the error. I would venture to guess maybe the variable string it is trying to call is not correct for some reason??

PS - I tried a couple of iterations, and also did an exact copy/paste into the processor just in case I misspelled or something, but no dice.

Please review!

Thank you.

Nick

[SeanDa]

Remove the CALL from the program block. Somehow that slipped in there even after I removed it from the original script.

[NICKKINSMAN]

That did it, works like a charm now.

For reference, the new program block section is:

Dim finishPass
finishPass = Lathe_GetFinishNumberOfCuts()
Lathe_SetReturnString("Q"&finishPass&"")

Q is the variable for final number of passes that Mach 3 needs.
Here is the threading string from the processor as well, referencing 'program block 1' which is where the transform resides in my case. Be sure to adjust the referenced lines to the correct variable descriptions in Mach3 for those that are adjustable by procesor lines.

87. Start of thread (G76) cycle
n,"G76",thread_x2,thread_z2,thread_lead,thread_fir st_cut,thread_angle_in,thread_machine_allowance,th read_last_cut,program_block_1,"L360 (Remove if no chamfer)"

Finally;

The 'first cut amount' line needs to have a '.' included after the variable due to a bug that does not pull in the decimal place, here's the example:

792. Prefix for thread G76 first cut amount? "H."

Thanks again, great support Sean.

[SBC Cycle]

Remove the CALL from the program block. Somehow that slipped in there even after I removed it from the original script.

Hey Sean, what IS the proper usage of the "CALL" function? Is that a VBScript function or a reserved BobCAD API thing?