I can't seem to get my rotary to follow my mastercam

[Rafael Rivera]

HI guys here is my delema

I have a Dekel Maho DMU 60T,basicly a 5 axis with a rotary as my c axis and the head moves 15 to

-90 degrees.What I'm trying to do is mill the outside of my part using the axis substution in mastercam,but my rotary does not follow what i see in my computer,my post guy says he doesn't understand why it doen't work ,does anyone know what the code should look like,just milling a simple square using my rotary,any help would be great!

[Allan Brown]

Rotary substitution is rarely hooked up for a machine config like that. It's typically a 4-Axis technique for parts with datums inline with the rotary center. Specifically for your machine, 5-Axis is done in M128 (TNC) or G141 (Millplus) mode, which is actually data mapped to the top, with the right rotary angles output.

 

If you can do it with a multi-axis toolpath instead, that would be mint.

 

However, our DMG posts should be handling that programming style, but mapping the moves into the right code format.

[crazy^millman]

That or just use C-planes with each side of the part you are machining. A pain to program this way I know we face this all the time when doing milling on Mill turns. Sometimes you have to machine part of the feature with one C-plane and then another part of the feature with a different C-plane so you can keep it working inside of the working envelope of the machine.

 

HTH

[Rafael Rivera]

Thanks for your help

[Rafael Rivera]

I tried maching my part using the muti axis ,but rotary doesn't want to engage,what it does try to do is machine around the part in 3 axis like,I am trying to machine around my part but I don't don't have enough travel,but if I'm able to use the rotary I would be able to machine around the part.

[Guest]

Rafael,

 

Has your reseller been any help for you on this?

[Rafael Rivera]

THEY gave me a couple of fixes but it still not working,that's why I'm trying this route,I even tried emailing and calling DMG and still no fix and no reply

[Greg_J]

Figures! Thats DMG for ya!

[Allan Brown]

Depending on the control TNC or Millplus there are M-Codes for the tilt ranges:

 

M50, M51, M52 for TNC

M56, M57, M59 for Millplus

[Post dept]

Hello Rafael,

 

Are you using M128 (TNC) or G141 (Millplus) during your axis sub?

 

I have nothing but good things to say for the service that DMG provides....

 

Brett

[Rafael Rivera]

Hi Brett,

 

I have a Heidenhain Millplus IT,I tried using the G141 it didn't work for me,then I tried the M128 it finally works (yahooooo !!!),It has to be done only with the part (x,y,z)zero off the center of the rotary like you said in one of your earlier text,and the cutter comp in the computer and it works fine

 

Thanks for all the help and support

Rafael Rivera @inlineplastics

[Post dept]

OK cool. That's often the missing link. Coordinates work differently inside the TCP functions so if something isn't working that's often the ticket.

 

BUT, M128 is a TNC function.....not Millplus. M128 should give you an alarm in Millplus.

 

Try with neither of the codes, and datum on rotary centre.

 

The version of the post that I have for you here does not have axis sub turned on.

[Rafael Rivera]

I got this post from MacDac,They were trying to make it work for me,but we couldn't figure out why it wouldn't for me,so i tried with DMG and never got a call back,but the M128 seemed to be the missing link,the G141 just made the tool follow the same point on the rotary for me,I don't know why ,I just know it does work

 

THANKS AGAIN