How To Edit Mastercam Post?

[Bala]

Can Anyone Help Me To Modify The Mcam Post.i Don't Know Anything About Modifying The Post.for Example On Cincinati 950 Mill When I Do Tapping Cycle Always Give Me A G00 In Front Of G84.how Do I Get Rid Of It.on Which Windows Program Do I Have To Open The Post To Modify.thanks

[Matt Berube]

You could open the post in many different programs.

It will open in "notepad", any .nc editor, etc. I like to use the Mastercam X Editor for looking at posts because the way the colors are displayed can be very helpful.

I don't know much about posts though so I can't help with your specific problem.

#1 most important thing about editing your post : SAVE A BACKUP COPY BEFORE YOU START !

[leif]

What version Mastercam are you using? Have you contacted your reseller? They will usually do post mods either free or real cheap. Try looking at WWW.EMastercam.COM.

[Alex_Cole]

When editing Mastercam posts make sure you do not open up the file in a program like word where it will format the text. This will make the post un-usable in Mastercam. Use notepad like mentioned before. In Mastercam you can use the following to open your post in an editor.

V9 system. File/Edit/Other. Then browse to and select your post.

X system. File/Edit-open external. Browse to and select your post.


I highly urge all Mastercam users to go to there local dealer to get this work done first. Unless you are experienced in what you are doing with a post you can really mess things up and could crash your machine tool. Please test all post work throughly and carefully. If you cannot find someone to help then contact me and I can help you find someone in your state/country who can help you.

I am not shure what your post looks like and that will have an affect on how it is to be edited. I also am not sure but it sounds like you are saying that the G0 is on the same line as the G84 cycle. If this is the case then look for the following in your post. This is just an example and your post may vary.

Here is the logic for ptap in the X2 MPFan.pst file

ptap$ #Canned Tap Cycle
pdrlcommonb
result = newfs(17, feed) # Set for tapping Feedrate format
pcan1, pbld, n$, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,
prdrlout, *feed, strcantext, e$
pcom_movea

Now the variable *sgdrill (the * just forces the value to be output) is the variable that outputs the G84.

*sgdrillref outputs the G98 or G99 from the selector table in the upper portion of the post processor.

If in your post you see a variable that looks like this *sgcode, or just sgcode without the * then this is the variable that is outputting the G0 in your program. If you see this it may look like the code below.

ptap$ #Canned Tap Cycle
pdrlcommonb
result = newfs(17, feed) # Set for tapping Feedrate format
pcan1, pbld, n$, *sgcode, *sgdrlref, *sgdrill, pxout, pyout, pfzout,
pcout, prdrlout, *feed, strcantext, e$
pcom_movea

Notice the *sgcode, remove the "*sgcode," from this line and it should remove the G0 from your output. Again this may differ from your post so be careful.

Again I also urge you to contact your dealer to get this fixed. They should be able to fix this very quickly.

Thanks and I hope this helps.

AC

[Mike Mattera]

Does the G0 Matter? Did your control complain?

It's possible you cant have 2 G's on the same line, but it does have to be in G0 to rapid between locations. You might want to move the G0 to the line before the Canned cycle.

pbld, n, sgrapid, e

Something else you might find useful....
http://www.mmattera.com/mastercam/index.htm

Mike Mattera

[rgammage]

Hello Bala

I used to be a Mastercam reseller so .....
1 if you can describe what MC gives you and
2 what you would prefer
and 3 email me the PST file you are using I will try and alter it for you.

Regards

Richard

[MicroMill]

Make sure you copy your original post to something like *.pxt in the event that your inadvertantly wack some code out of your post.

Alex Cole was very much in the ball game with his reply. If you have a good working relationship with your Mastercam dealer, they can turn you on to the Mastercam Post Processor Programming Guide (.PDF) that will step you through the basics.

[ezdiani]

hai everyone....i'm new
hope everyone can help me if i have a problem....
i'm pogrammer at my factory...so please help me....

[joecnc1234]

Hi all I have to say is save a backup of your post then have fun messing around with your test file. It took me a couple of days of screwing around to get my posts how I like them. Just look for things in the post file that reference the areas your trying to change remove or change the things you want to change and repost to see the results only change one thing at a time and sooner or later you will have what you want the satisfaction of doing it yourself is great plus you don't have to wait for anyone else to help you. btw I use File/edit/pst to get default mc editor

[Mike Mattera]

Richard, who did you work for, 4D?

We might have met at a Dealer meeting in 1998. It was in Cape Cod or something like that. I was with ShopWare. We were at a bar across from the hotel having a beer with Stewart Roney & you (i think). Except we weren't staying at the hotel. We had a room at a local B&B. I dont know why.

Mike Mattera

[rgammage]

Hello Mike

I was one of their dealers and did not visit the States. The guy with Stuart was probably Nick Hinde the Technical Director.

Regards

Richard

[jonesr]

I work on an old Kitamura mill at work with an added 5th axis. Im just getting into mastercam as well. Are there any guides or tutorials on modifying a post file for your machine ? or is it just a matter of knowing how your machine likes the code arranged in program files ?