Cutter Comp Value D

[CHRIS2010]

I have a problem with the cutter comp value D when I post the same program for different machines.

I use D=H+40 for most of the machines. However, I sometimes have to repost the same program for other machine which can take D=H.

I try to make changes in the box of row "Add to tool" and colunm "Diameter" in the machine control page under the tool tab, but

nothing change unless I change the value in the box of " Dia. Offset" in the tool parameter. Changing the values in the tool

parameter is not a correct way, I think, and takes a lot of time.

 

Anyone can help me on this issue, please.

 

Thank you in advanced.

[Guest]

If I understood you correctly, you have different control def with different tooling numbering schemes.

 

If so, when you change and need to repost, try renumbering your tools to pick up the new settings

[CHRIS2010]

Hi John,

Basically, I would like to set up the machine def in such a way when I post the program, I will have whatever D values

(D1 or D41 for T1 etc) without change anything in the tool parameter.

[spade117]

One of my biggest complaints to the scheduling department. Same issue here...if you open the parameters and just re-click on the tool, it will update to the proper D# for that control.

 

What you want to watch out for is it can change other settings in that tool if you have default values that are in your tool library and the coolant, peck and step tab is checked. It will revert back to standard settings if you have changed anything else.

[Leigh @ Kodiak]

I had our post modified so that a user input will determine if D=H or if D=H+40. This way I never have to worry about switching anything, just simply repost the program.

[Bryan Johnson]

"I had our post modified so that a user input will determine if D=H or if D=H+40. This way I never have to worry about switching anything, just simply repost the program."

 

+100

 

Anoter benifit to letting the post handle the "H" and "D" values is not having to worry about them being wrong, and simply focus on the tool number when writing the programs.

[spade117]

I had our post modified so that a user input will determine if D=H or if D=H+40. This way I never have to worry about switching anything, just simply repost the program.

Do you know exactly what was modified?

[Bryan Johnson]

Spade,

You would need to add logic to the postblocks where tlngno and tloffno are output.

Below is an example of modified post blocks.

variables h_offset and d_offset need to be initialized elswhere.

I can email you an example post.

 

p_tlngno # output tool length offset

h_num = t$

if h_offset = 0, *h_num, !tlngno$

else, *tlngno$

 

p_tloffno # output tool dia offset

if d_offset > 1, d_num = t$ + d_offset

else, d_num = t$

if d_offset = 1, d_offset = tloffno$ #set from NCI

d_num, !tloffno$

 

 

[CHRIS2010]

Spade,

You would need to add logic to the postblocks where tlngno and tloffno are output.

Below is an example of modified post blocks.

variables h_offset and d_offset need to be initialized elswhere.

I can email you an example post.

 

p_tlngno # output tool length offset

h_num = t$

if h_offset = 0, *h_num, !tlngno$

else, *tlngno$

 

p_tloffno # output tool dia offset

if d_offset > 1, d_num = t$ + d_offset

else, d_num = t$

if d_offset = 1, d_offset = tloffno$ #set from NCI

d_num, !tloffno$

 

 

Hi Brian,

Do you have any idea for the tab "Tool" under the control definition.

Please look at the attach. I think that is this page for, but doesn't help.

Control_def.pdf

[Bryan Johnson]

using the options in the Control file will work for creating a new program, but are not much help when you want to post to a different machine that used different rules for offsets.