[facegarden]

Yeah, it looks like you're going to need to post the file or send it directly to me. I can't look at it until tonight. PM me if you can't post it for whatever reason and need my email address.

Yeah, looks like. I tried the tip above too to no avail.
Here's the file.
-Taylor

[Donkey Hotey]

It works on mine. I did a 2" translate, 4 copies, to the right and it posted:

G54
G55
G56
G57

I saved it and reposted it here. See if it doesn't work now.

[Geof]

Maybe it will make you feel good to know that because of this thread when we met with the MasterCam guy recently I was able to ask questions that made it appear I knew far more than I really do about the multiple work zero output. I also was able to ask questions about things like trochoidal machining and face peeling.

So you guys should feel thoroughly brain-picked.

When we placed the order he asked my Production Manager how many MasterCam Tee-Shirts we wanted. The answer was that if we didn't want to play favorites it had to be none or sixteen so we could give one to each guy; so now we have sixteen $1,000 tee-shirts and they threw in two MasterCam seats as an extra.


P.S. Haas Apps you owe me about 1200 Haas Tee-Shirts.

[Donkey Hotey]

That's good news, Geof. If I read enough of your posts, I might someday take "CNC nOOb" off of my signature line.

[Geof]

Should I post a picture of me in a MasterCam Tee-shirt?

[tobyaxis]

Should I post a picture of me in a MasterCam Tee-shirt?

Only if it says Mastercam X4

[facegarden]

It works on mine. I did a 2" translate, 4 copies, to the right and it posted:

G54
G55
G56
G57

I saved it and reposted it here. See if it doesn't work now.

Yeah, I'm really starting to think this is an issue with my Post, as that file doesn't do it for me. Grr... Are you using the generic HAAS 3 axis post or something else?
Thanks,
-Taylor

[Donkey Hotey]

Yup, standard Haas post. What version of Mastercam are you running? I've made some minor tweaks to my post so I'm not sure if I'd be comfortable recommending it (I don't remember what I did--it's been awhile).

You opened the file and didn't change anything, right? Are you SURE that it didn't create the extra work offsets? I'm assuming that you searched for G54 and found it multiple times. That's correct since it's going to do one operation at G54, then G55, G56, G57, then start over with the next op: G54, 55, 56, etc.

Did you also search for G55, G56, etc?

[facegarden]

Yup, standard Haas post. What version of Mastercam are you running? I've made some minor tweaks to my post so I'm not sure if I'd be comfortable recommending it (I don't remember what I did--it's been awhile).

You opened the file and didn't change anything, right? Are you SURE that it didn't create the extra work offsets? I'm assuming that you searched for G54 and found it multiple times. That's correct since it's going to do one operation at G54, then G55, G56, G57, then start over with the next op: G54, 55, 56, etc.

Did you also search for G55, G56, etc?

Yup, I found no G54, G55, etc in the posted file at all. I have also made some changes to my post I don't remember (trying to learn things and all), let me see if I can find my original unmodified machine definition and post and try posting with that.

Thanks so much for helping!
-Taylor

[facegarden]

Hey sorry I haven't been back here, work has been busy and all.
So I'll have to keep looking, I don't think I was able to locate my unmodified post so I'm not sure if my issue is the post or not. Do you mind sending me your post just so I can verify it's not something else? I know you said you don't recommend using it, I just want to make sure my post is the issue.
Thanks,
-Taylor
You can send it to my email at tlalexander <ignore this part> ~at~ gmail "dot" com

[cadcam]

facegarden, what version of Mastercam X are you running as this makes a difference on the post. I wanted to share but need exact version or the post wont work.

[facegarden]

I just have X1.
-Taylor

[facegarden]

So, it seems I can't get anything to post with multiple work coordinate systems.
I've tried just making two drill points and setting each one to its own WCS, but when i post, it still just acts like I had set them both in the same WCS.

Is that more likely in my post, or in my machine or control definitions?

Attached is what I have under the "work system" tab in my control definitions, if that makes a difference.
Thanks,
-Taylor

[Donkey Hotey]

Did you get my email? I sent you the post. Have you tried it?

[facegarden]

Did you get my email? I sent you the post. Have you tried it?

Ah! Sorry, i get so many e-mails that sometimes I miss things!

Well turns out your post works!

Furthermore, I was able to get my post to do it!

We have slightly different functions for
"pwcs #G54+ coordinate setting at toolchange"

Yours is:

pwcs            #G54+ coordinate setting at toolchange
        sav_frc_wcs = force_wcs
        if sub_level$, force_wcs = zero
        if workofs$ <> prv_workofs$ | (force_wcs & toolchng),
          [
              if workofs$ =  -1,workofs$ = 0
              if workofs$ < 19, g_wcs = workofs$ + 54
          else, g_wcs = workofs$
              if  (workofs$ > 5) & (workofs$ < 19), g_wcs = g_wcs +  50
              if (g_wcs < 54) | ((g_wcs > 59) & (g_wcs < 110)) | (g_wcs > 122), pwcs_bad
          else, g_wcs
         ]
        force_wcs = sav_frc_wcs
        !workofs$

Mine was:

pwcs            #G54+ coordinate setting at toolchange
      if mi1$ > one,
        [
        sav_frc_wcs = force_wcs
        if sub_level$, force_wcs = zero
        if workofs$ <> prv_workofs$ | (force_wcs & toolchng),
          [
          if workofs$ < 6,
            [
            g_wcs = workofs$ + 54
            ]
          else,
            [
            g_wcs = workofs$ + 104
            ]
          if workofs$ >= 0 & workofs$ <= 25, *g_wcs
          else,
            [
            if mprint(swcserror, 2) = 2, exitpost$
            ]
          ]
        force_wcs = sav_frc_wcs
        !workofs$
        ]

I noticed mine had the "if mi1$ > one" condition. The rest of my WCS code seemed to be sensible, but yours didn't have that if statement. I wondered if my post was failing that IF condition and never setting the WCS, so i removed the if statement and everything works!

I have no idea what that will do to other things, I am going to need to start looking into what all this stuff in the post means, but for the record and in case it wasn't clear, I ended up with that section of my post like so:

pwcs            #G54+ coordinate setting at toolchange
      
        sav_frc_wcs = force_wcs
        if sub_level$, force_wcs = zero
        if workofs$ <> prv_workofs$ | (force_wcs & toolchng),
          [
          if workofs$ < 6,
            [
            g_wcs = workofs$ + 54
            ]
          else,
            [
            g_wcs = workofs$ + 104
            ]
          if workofs$ >= 0 & workofs$ <= 25, *g_wcs
          else,
            [
            if mprint(swcserror, 2) = 2, exitpost$
            ]
          ]
        force_wcs = sav_frc_wcs
        !workofs$

The only real thing I noticed is that mine only allows 6 consecutive WCS's above G54 while yours allows 19, which my machine wouldn't support, I don't think.

Anyway, anyone know what I deleted?
Thanks!
-Taylor

[Donkey Hotey]

consecutive WCS's above G54 while yours allows 19, which my machine wouldn't support, I don't think.

I don't know what year your machine is but you have G54-G59 for your first offsets, then you may have G110-G129 as well. I'm not sure when Haas introduced those extra work offsets.

[Geof]

.....then you may have G110-G129 as well. I'm not sure when Haas introduced those extra work offsets.

These have been available at least from 2001.

[mikefalkner]

Donkey Hotey,

Thanks for your posting on 10-25-2008, 10:41 PM. This was exactly what I was looking for. Your old posting really helped me.

Again, THANKS!
Mike