Generic mill with mpfan A axis switch

[Chris Rizzo]

So out-of-the-box default generic mill mmd. turning off the A axis combo's in machine def (yes both places), and A still posts. I use this switch with all my haas posts and it works. I'm back into v9 era with doing it in the post.

[Colin Gilchrist]

Chris,

 

With 'MPFAN', there is a switch inside the post:

 

read_md : no$

 

This has been there since the start of the Mastercam X platform. Setting this switch to 'yes$' will cause MPFAN to read the Machine Definition settings, instead of only reading the variables in the Post.

 

If you use 'Generic Fanuc 4X Mill' post instead, this Post reads the Machine Definition automatically. (Select 'Mill 4X VMC' or 'Mill 4X HMC' MMD file).

[Chris Rizzo]

Thx Colin, I'll try not to shoot the messenger...

 

Well the implementation of the mmd/control setup was supposed to eliminate going into the post, right? So now, you STILL have to go into the post. But now telling it to make the machine def. functional, then go into the machine def and make your adjustments.

 

If I'm going into the post, I'll just turn off rot_on_x and be done with it!

 

The entire mmd / control setup is such a needless headache. (Recently read a few dealers who spends 90% of their tech support time on mmd issues)

 

 

If you use 'Generic Fanuc 4X Mill' post instead, this Post reads the Machine Definition automatically. (Select 'Mill 4X VMC' or 'Mill 4X HMC' MMD file).

 

The problem with THAT is the default arc type is set to radius! What's up with that?

 

 

thx for the reply Colin, just sendin' that stuff up the flag pole.

[K2csq7]

The entire mmd / control setup is such a needless headache.

 

Wondering why these were ever implemented.

[Colin Gilchrist]

Chris,

 

You do not have to go into the Post, if you use 'Generic Fanuc 4X Mill', instead of 'MPFAN'. These posts are basically identical, except one has a 'read_md' switch, the other does not.

 

If all you wanted to do was switch from 4 Axis to 3 Axis output, I'd recommend replacing the Machine Definition file with 3 Axis one, (or create an Axis Combination that is 3 axis only).

 

I just checked the 'Generic Fanuc 4X Mill.Control-6' file, and the default Arc settings are Delta Start to Center. When I checked the 'Generic Fanuc 3X Mill.Control-6' file, I did find that the defaults were set to Radius.

 

Thank you for letting us know about the Arc Defaults for the Generic Fanuc 3X Mill. I'll go in and edit the defaults for that Control file so that all the Arc Center defaults for the Fanuc Control files match.

 

Thanks,

[Chris Rizzo]

Ok, so to get basic 3 axis fanuc code with ijk's you cannot post and go, someone has to do one of following:

 

-Mill Default/mp fan, requires going into post switching read_md : no$m, and then turning off A in mmd

 

-Mill 3 x /Generic Fanuc 3x, requires going into control def and switching to delta start to center.

 

-Mill Generic 4 x / Generic Fanuc 4x, requires going into machine def and turning off A axis combos.

 

 

Correct me if I'm wrong, but a total entry-level-new-customer who wants to post the most common type of fanuc code, needs this (moderately) advanced knowledge.

 

 

Since I've got your ear Colin, any word on inverse time with 2dhst toopaths?

[mayday]

I'm felling a little dizzy myself

Dont ask about the coolant Chris

[Chris Rizzo]

Reason I'm on this so hard, I've got a class of 15 new users who just want the most basic fanuc code and are having to go through this. Not only in the classroom, but then remember it all when they go back to their shops.

[K2csq7]

I've got a class of 15 new users who just want the most basic fanuc code

 

Make sure you hand out a local reseller's business cards...

 

-Mill 3 x /Generic Fanuc 3x, requires going into control def and switching to delta start to center.

 

I'd go with this one for your class (but skip changing to I,J,K's).

R's are about as basic as it gets.... Is there something holding you to the I,J,K's? (curriculum or something?)

[Colin Gilchrist]

Ok, so to get basic 3 axis fanuc code with ijk's you cannot post and go, someone has to do one of following:

 

-Mill Default/mp fan, requires going into post switching read_md : no$m, and then turning off A in mmd

 

-Mill 3 x /Generic Fanuc 3x, requires going into control def and switching to delta start to center.

 

-Mill Generic 4 x / Generic Fanuc 4x, requires going into machine def and turning off A axis combos.

 

 

Correct me if I'm wrong, but a total entry-level-new-customer who wants to post the most common type of fanuc code, needs this (moderately) advanced knowledge.

 

 

Since I've got your ear Colin, any word on inverse time with 2dhst toopaths?

 

Hi Chris,

 

Yes, you are correct about the steps necessary to output Fanuc IJK code for a 3 Axis machine. I did fix the Default settings for Generic Fanuc 3X Mill.Control-6, so that you will not have to do one of those steps in the future. Unfortunately, this change won't make it into Mastercam until the next time we do a build. This change will be included in the next release of Mastercam though (so you'll see it in Beta).

 

I updated your thread in the Beta Forum with information about the 2D HST Inverse Time issue.

 

Thanks,

[Chris Rizzo]

Thanks Colin! Great service

 

 

R's are about as basic as it gets.... Is there something holding you to the I,J,K's?

 

Arc checking with centerpoints on ijk's.

[Bill Henderson]

I use the Generic HAAS 4 machine def. To rid myself of the A posting I went to machine def and in the machine configuration window I disabled the VMC A axis under the table group. This eliminated the posting (a axis posting). With the HAAS I still get IJKs.

 

I do not remember having to switch it in another place although it just may be my mind is going.