Missing g1 code

[archer]

Hello,

This is my first time asking a question so please be kind.

We are currently using ver. 9.1 at work, and we have come across a problem when we machine surfaces. What is happening is when we have two surface finishing parallel paths, using the same surfaces, but different tools, the posted program is missing a g1 code after the tool change. This only happens when we post both operations back to back. If we post just the second one, it places it in there. If we post another operation (i.e. contour) between the two parallel operations it places the g1 in the proper place.

We are currently running a Fadal 6030 with the mp32 control and also a Fadal 4020.

Any help please.

 

Dennis Archer

Plastic Ingenuity

Oxford, NC

[CAM-mando]

never mind ...

 

[ 05-13-2003, 09:20 AM: Message edited by: CAMmando ]

[Guest CNC Apps Guy 1]

Hello Dennis,

 

Which post are you using and has it been modified in any way?

[chris m]

+1 on what James said

 

Could you post a (simplest possible) file that exhibits the difficulty that you're having to the ftp site so that we can look at it?

 

C

[archer]

We are using a modified mpfadal post. Everything has been working fine with it, and this has just seemed to start happening since we upgraded to v9.1 from v9.0sp1. P.S. It doesn't happen all the time, (i.e. different surface, but same operations, it will work fine???)

 

Here's the shortened program:

 

After first tool runs...

 

N109Z.1F100.

N110M9M5

N111G0Z0H0

N112T5M6

N113M1

N114M3S6500

N115E1G0X5.4076Y2.7004 <------ last g code present

N116H5Z.1M8

N117Z-.0934F10. **** <----- there should be a G1 here???

N118X5.4052Y2.7029Z-.1051F55.

N119X5.401Y2.707Z-.1118

N120X5.3969Y2.7111Z-.1051

N121X5.3944Y2.7136Z-.0933

N122Z-.087

N123X5.3868Y2.717

N124X5.3871Y2.7167Z-.0896

 

Continues on....

 

Thank you for the quick interest in this.

 

Dennis Archer

[Trevor Bailey]

Archer,

 

Did you update this post to run with your current version? I have a very good Fadal post that I can send you if you would like.

[gms1]

[ 05-13-2003, 12:26 PM: Message edited by: gms1 ]

[archer]

Trevor,

I didn't realize that the post also needed to be updated, because we have been using it since ver. 8.0 was out. If you could send me that post to try, it may help.

 

Thank you,

D. Archer

[Trevor Bailey]

Before I send the post to you, try using the UPDATEPST c-hook to update your post to the current version you are on. This should take care of your problem. If you still have issues, contact me and I will be more than happy to walk you thru the process to get you running smoothly.

[archer]

That still doesn't work, I updated the post like ya said, but still no G1.

[Trevor Bailey]

Archer,

 

Check your e-mail.

[Nominal]

Just for laughs do a search in your post for G0.

I wonder if there isn't some code in there that doesn't use sgcode and forces "G0". That would cause the post not to output another G1 where you think it should have.

[archer]

Hey,

I got it to post a G1. It seems that the post isn't messed up. We had the clearance box checked and set at .100, the retract box checked and set at .100 abs., and the feed plane set at .100 abs. It seems that if you change the retract height to something larger than the feed plane, or have the feed plane on inc. then it will post normal (w/ a G1). If you have everything set at .100 and abs. some reason it will not post a G1.

Any reason on why this happens? For know,we can set everything to avoid it in the furture though.

 

Thanks

Dennis Archer

[Trevor Bailey]

Archer, disregard my e-mail then. This is exactly what I wanted to check. Glad you found the error.

 

Good Luck.