Hello

I've just been modifying a basic post-processor to suit the 1985 Denford Triac mill I have access to. I've now got everything tweaked to my satisfaction except for one thing. For feed rates in the X and Y, the triac requires FX to be defined, for moves in the Z, FX must be defined - e.g.

G01 X150 Y50 FX100 Z150 FZ50

However, what the post produces is :-

G01 X150 Y50 F100 Z150 F50

If I change the function defintion to FX then it replaces F wih FX
all the time. Mastercam seems to know the difference between feed
and plunge rates - but assigns the same variable to them both. Is
there a way that I can get the post to insert FX and FZ as
appropriate ?

Any help would be great

Thanks

Dave

Davidimurray, I've had to configure a post myself. If you want to post/send the actual post file, I'd be more than willing to take a look and see if I can help.

And if I can't help, there's several that will also be of assistance....guaranteed. :)

*edited because I can't read*

David, what version of MC are you using?Send me the post please, and I fix for you.

Regards

Daniel

Hi everybody - thanks for the offers of help. I'm using MC 9. Please find enclosed the post file. It works just fine except that X and Y moves should be associated with a feed FX and Z moves should be associated with an FZ feed. At present all of them output FX and then manually go through and change the required ones to FZ.

Thanks Again

Dave

I was sitting here going through this, and got to thinking about something. How do you input 2 different feedrates in mastercam? I've never seen the option of having a feed for X and/or Y and a different feed for Z.

You can actually have 3. The first is for x & y. This is on the define tool page as feedrate. there are also plunge and retract feedrates available there

Mark

Doh! Didn't even think of it that way. Now that you mention it, the plunge rate could be for X Y and Z (if ramping).

But I don't know of any place to define 2 different feedrates for use on the same line.

It's up to the post to take the 2 types of feedrate and manipulate them so you get the desired result. Every post I've ever worked with just has one feedrate and whether it's used with z or x & y (or x, y & z as in the case of helical) determines if it's plunge or contouring. I've never seen one to output one such as asked for, but I'm sure it can be done. Might take a crack at it myself

Mark

Hi David, I´m working in your post.I don´t read your reply before because a long holiday that we have here.But now all it´s Ok again.I already solve the problem.I´m testing now.Hang in there!!!!

David, I put in attach with this reply your post.
I create a rule in pst that when you have a move only in Z, put only FZ, when you have a move only in X or Y or both, put only FX, and when you have a 3 axis moves (XYZ) or X or Y move combined with Z (XZ OR YZ) the post put FX after X/Y values and FZ after Z value.
Try and report to me your results.

Like below:

G90
G71
G54 X0 Y0
M06 T2
M00
( CHANGE TOOL )
G98
M03 S2800
G00 X-15. Y5. Z2.
G01 Z0. FZ215. <- Only FZ
G01 X-20. FX230. <- Only FX
G03 X-25. Y0. CX-20. Y0.
G03 X0. Y-25. CX0. Y0.
G03 X25. Y0. CX0. Y0.
G03 X0. Y25. CX0. Y0.
G03 X-25. Y0. CX0. Y0.
G03 X-20. Y-5. CX-20. Y0.
G01 X-15.
G00 Z200.
G00 X-102.186 Y62.554
G00 Z50.
G00 Z2.
G01 Z0. FZ220.
G01 Y57.554 FX111.
G03 X-97.186 Y52.554 CX-97.186 Y57.554
G01 X-89.686
G01 X91.685 FX110. Z31.98 FZ110. <- 3 axis move - FX and FZ respectively
G01 X99.185 FX111.
G03 X104.185 Y57.554 CX99.185 Y57.554
G01 Y62.554
G00 Z50.
M06 T3
M00
( CHANGE TOOL )
M03 S3000
G00 X-3.922 Y-66.05 Z-.107
G01 Z-2.107 FZ124.
G01 Y-64.52 FX123. Z-.126 FZ123.
G19 G02 X-3.922 Y-57.199 Z8.278 CX0. Y-2.138
G02 X-3.922 Y-49.89 Z13.5 CX0. Y-36.916
G02 X-3.922 Y-41.313 Z15.459 CX0. Y-41.313
G02 X-3.922 Y-39.686 Z15.392 CX0. Y-41.313
G02 X-3.922 Y-31.878 Z13.972 CX0. Y-42.853
G02 X-3.922 Y-23.884 Z11.555 CX0. Y-107.71
.....

Hope that helps.If work let me know.

Kind Regards

Note: Sorry my Bad English.

Hi camfun

I've run the post a couple of times and all appears well. I haven't had time to test on the machine yet as I've been adjusting the gibs and sorting out a couple of other problems. As soon as I run a test (hopefully in the next few days) i'll let you know how I got on.

Finally I'd just like to say a BIG BIG thanks to you for all your help. You've made me a very happy man.

Thanks Again

Dave

Hi Camfun

Ran a test program last night and everything worked perfectly.

Thanks for the help - much appreciated

Dave

I stay very happy to can help you, David.
If you have any problem with posts for mastercam, I will stay very glad to help.
Any problem, contact me by mail.

Your brazilian friend.