You are not logged in.
Pages: 1
Using Vericut 5.4.3 and simulating a Fanuc 15m, I have usually seen Block Skip (i.e. slash: "/") as the first character of the block. However, it seems that this character may appear after the block number. The Fanuc manual says if the slash is placed other than at the beginning of the block, that the information from the slash to the EOB is ignored, while the information before the slash is effective.
Does anyone know how to tweak the fanuc15m.ctl file to accomplish this?
Offline
I wouldn't put / at the end of block.
/ at the sart of block will skip this line. If the block skip button is active on the controller.
I have / on the 5-axis machines for the rotary home at tool change.
So if the operator wants to resart at any Toolchange position he can and not have to home the A and B axis's.
By the way I can't get my Vericut to skip these lines (/) still homes the rotary every tool change?I have / as the block skip character
and apply switch value Immediate?
Cheers
Offline
G'day, mate!
I should have illustrated my question with the situation I have encountered. First, I have always placed the "/" character at the beginning of the block. But, in this case, I have inherited a folder of programs from someone who retired, who never used Vericut, and I am using Vericut when I make minor changes to his jobs. (Minor changes do not include reformatting every line, esp. when the nc files are large.) So an example is:
N300 /G65 P9853 B1. T17 S.7500
or
N450 /#2007=5.350
When I review the debug file, it seems that Vericut does not stop when it encounters the "/", as the Fanuc manual says that the controller will.
Anyway, I will keep chipping away at this.
Ta
Offline
I wouldn't put / at the end of block.
/ at the sart of block will skip this line. If the block skip button is active on the controller.
Cheers
David,
If someone asks a question on how to get Vericut to do something, please don't suggest changing their programs.
Look at >Setup >Control >Settings >Tooling >Tool Change retract method and
>Setup >Machine >Settings >Tables >Add/Modify >Tool Change retraction/Tool Change Location
Robert,
I have seen examples of what you describe in programming manuals:
N100 G0 X1. / Y2. M8
The X will move, but the Y and M8 will be ignored.
Have you contacted CGTech support directly? I have found that you will get you answers much quicker.
Good luck,
Al
Austin NC APT administrator.
Custom configure GPost for Pro/E,
and other ANC applications.
Offline
To your question: Have I contacted CGTech?
I have not contacted them yet. I wanted to see what sort of answer I could receive from other users first. I am going to wait until next week. If I don't hear by then, I will submit an email to CGTech support (heads up). They always seem to do a pretty good job for me.
L8er
Offline
Robert- have you tried the "BlockSkipAnywhere" macro? The notes below came from the on-line Help docs in the macros seection. I tested here and it behaved the way you have requested. --Gene
BlockSkipAnywhere— Allows the block skip character to be anywhere in the block. This macro should be called during the "Reset" event with an Override Value of "1". When active, the block will be processed up until the block skip token is read. The remainder of the block will then be skipped.
NOTE: This macro should only be used when the block skip character can not be interpreted as anything except a blockskip character. It should not be used when this token could also mean divide.
Offline
Gene:
Holy dooley! Good onya, mate!
I'll have to check the probing set-up logic to see if we are averaging the probe results.
Cheers,
Robert
Offline
Pages: 1