Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Post processor needed

cnc girl

By cnc girl,
in Industrial Forum

 Share

Recommended Posts

cnc girl Newbie

cnc girl

Posted
Posted

Hi gang,

 

New to the group, I will ask mastercam monday if I cannot find a post from you guys.

 

Looking for a post for an Emco TM02 VMC. The post avail here at the education div. is for the lathe. I need one for the mill. Any help would be appreciated. Or if anyone has a post processor book avail (teaching you how to modify posts) I would gladly buy it. I have send a request to mastercam to see if they have one for sale too.

Currently trying to modify avail post with no luck

 

Thanks for any help

 

CNC girl

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

Well we have all be asked not to do that for 10 posting so they flame throwers are lit and waiting. J/K Have you looked on the Cd for the post you need. Take the cd and you have the ability to load post procossers only. You can load them all or just spefic ones. There you might find one close to what you need. The dealer is going to be the one to get you the PDF'S for the post modificating and it yes it will help. If you have spefic questions or sample NC code of what the post is doing and what you want we can help you get the post to your liking. I would also shoot an email to Mastercam with your school name and information along with the Sim number ans thin kthat can help you also. Hit Alt-V for the sim number no the matercam screen.

 

BTW welcome to the forum. cheers.gifcheers.gif

Link to comment
Share on other sites
cnc girl Newbie

cnc girl

Posted
  • Author
Posted

Thanks for the welcome.

 

I have loaded all the post from the CD and have been playing with other posts to see if they will work. For some reason my machine does not like any of the I's and J's in my arc command. Start or center point errors. I even tried a post that uses R's and still get an error. (Never mind all the other mods I have to make like spacing between the line number and the commands - need 2 spaces, or my line numbers have to be N0001, not N1)

 

bye for now

CNC girl

Link to comment
Share on other sites
HevyMetl Newbie

HevyMetl

Posted
Posted

I am by no means a post guru like some of the other members but check these lines in your post and see what is supported by you machine control.

 

arcoutput : 0 #0 = IJK, 1 = R no sign, 2 = R signed neg. over 180

arctype : 2 #Arc center 1=abs, 2=St-Ctr, 3=Ctr-St, 4=unsigned inc.

do_full_arc : 1 #Allow full circle output? 0=no, 1=yes

 

Do like I do and change a few things and save them as a seperate post and see how the output changes.

 

Welcome to the forum. This is best forum I have ever read and been a small part of. I read much more than I post, and I am sure someone will get you helped out.

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

Ok for the spaces look here in your post. BTW you should only use a editor for posts that does need to make it a txt to save it. Cimco is the one I use for my pst,txt,and any other things where I want the format and file to same the same as when I opened it.

 

code:
spaces    : 0      # Number of spaces between words

Change the 0 to 2 and see if that helps for that.

Link to comment
Share on other sites
cnc girl Newbie

cnc girl

Posted
  • Author
Posted

Wow, you guys are awsome.

 

Thanks for the CIMCO edit info.. I never new it existed. I will be working on it tonight. Changing the spaces and the arc commands.

 

Next question ... well maybe I should see if I can find it first. O.k. its still unclear...

- My tool change shows T300, I need it to read T0303.

- in my start up block it has a G90.. I need to remove it completely.

 

These are just a few at the moment. Gonna tackle the arc commands in a bit, gonna go out for a quick bite.

 

Any help again it just great

Bye for now

CNC Girl

Link to comment
Share on other sites
cnc girl Newbie

cnc girl

Posted
  • Author
Posted

Well its almost 11pm, changed alot of my post processor. Just stuck on a few. My tool shows T3 (not like I mentioned above) would like it to show T03 or even better T0303 and so on.

 

and my n line numbers - N1 should be N0001

 

I also need an additional space between the line number and the programmed line N0001 G00 Z0

should be N0001 G00 Z0

 

I Can send anyone my post processor if it helps. Been working long and hard, and I just can't figure it out. Comparing to other posts, just can't find the right clues.

Ronald .... I do not have that code option you pasted.

 

Thanks for all the help tonight. Got further than I thought, never expected to attempt this :-)

 

G-night

CNC Girl

Link to comment
Share on other sites
Christian Raebild Newbie

Christian Raebild

Posted
Posted

To get an extra space after the N number, you need to modify the format statement for n. It looks like this now:

 

fmt N 4 n

 

You need to change it to this:

 

fmt N 4 n " "

 

The number 4 might be a different number in your post processor, the number should not be changed. It is the bit added after the variable name 'n' that is important.

Link to comment
Share on other sites
BernieT Newbie

BernieT

Posted
Posted

To get that extra space needed, try replacing all the n, with n" ",

 

Look for this:

 

code:
 # --------------------------------------------------------------------------

# Toolchange / NC output Variable Formats

# --------------------------------------------------------------------------

fmt T 4 t #Tool No

and try changing the 4 to 5 or 6 or 7 (format statements)

 

I have not tried these changes so check them out carefully.

 

HTH

Link to comment
Share on other sites
Christian Raebild Newbie

Christian Raebild

Posted
Posted

To make it work when you hit 10 tools, and to make it work with N number like N0001 and N1234, you need to edit the format definition for the formats. A little explanation is probably in order here.

 

fmt T 4 t

 

The number four means format definition 4 is used for the variable t, so editing format definition 4 changes the output of the variable t. Format definition 4 probably reads something like this now:

 

fs 4 1 0l

 

If you change that to this:

 

fs 4 2 0l

 

Then you will get T01 or T12. However, that will alter all variables that use format definiton 4, so it might be necessary to make a new format definition to handle t. To do that you add a new line to the bottom of the fs format definitons, with a new number, and change the 4 in the format statement for the t variable to that new number.

 

To get n output like N0001 and N1234, you use the same method (either editing the format definition or making a new one), but here the format definition must read like this:

 

fs 12 4 0l

 

It might not be format definition 12 you need to edit or add, but the part after the 12 must read as I wrote it here.

 

Note: In the format definitions I wrote, it is the letter 'L' after the zero, not the number one.

Link to comment
Share on other sites
cnc girl Newbie

cnc girl

Posted
  • Author
Posted

Hiya!!

 

Hey Cristian (see your a night owl hehe) your the greatest! I would have never touched the fs area, would have never guessed.

The fs 12 4 0l i did have to change to fs 6 4 0l.

That is just unbelieveable. I changed the T03 as well.

Can't thank you enough.

Oh... I see your in Denmark, that explains everything!

Have a super day/night

CNC Girl

Link to comment
Share on other sites
Thad Enthusiast

Thad

Posted
Posted

quote:
Hey Cristian (see your a night owl hehe)

 

snipped

 

Oh... I see your in Denmark, that explains everything!

That's just one of the many great things about this forum. Everyone here has VERY QUALIFIED help 24 hours a day. We have forum brothers and sisters all over the world.

 

Thad

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...