MPMaster post help

[Leigh @ Kodiak]

Can anybody offer some insight as to how I would force the work offset output with every B axis rotation?

 

Thanks

[Chris Bloedorn]

Check to make sure your work offset is on...

 

either that or make sure that lock on first WCS is not on in the MISC values

 

 

 

[Leigh @ Kodiak]

I am currently getting correct WCS output at the first move after each toolchange. Say I have 4 operations on one tool,  what I need to happen is for the WCS to output on the B axis moves that are in each of the 4 operations.

[djstedman]

One way I can think of without messing with the post would be to force toolchange on each toolpath.

 

Since it outputs the work offset on each tool change, this would give you the work offset for each operation..

 

If that's not good enough I think you would have to look at your null toolchange block (ptlchg0) of the post and how to make it spit out the work offset on null toolchange.. 

 

I am sure it wouldn't be super hard to modify .. but then again.. just forcing toolchanges would be easier..

[Leigh @ Kodiak]

Unfortunately forcing tool changes is going to add a lot of time to a cycle that is already too long. I have been looking in the ptlchg0$ section, but get what I'm after quite yet.

[Chris Bloedorn]

it should post out the the work offset for each tool....try downloading the latest version here...

 

 

 

http://www.emastercam.com/board/files/category/5-post-processors/

 

 

[Chris Bloedorn]

OR check the general output settings in the post....make sure force_WCS  is set to yes

 

 

 

 

[CADCAM3D5AXIS]

^^^ Chris is there going to be a MPmaster for X9  mill and lathe ???

[Chris In-House Solutions]

There will be a mpmaster and mplmaster for X9.  We've wanted to make a couple of modifications to these files before putting them up online.  Currently the post team here is swamped which is why we haven't had time to make those changes and put the X9 files up.

 

 Leigh @ Race Face

I am currently getting correct WCS output at the first move after each toolchange. Say I have 4 operations on one tool,  what I need to happen is for the WCS to output on the B axis moves that are in each of the 4 operations.

 

Do you want the same work offset output for each B rotation or are you looking for it to output a new work offset each time the table rotates?

 

One thing to check is to make sure Misc. Integer #9 isn't set to 1 in the first operation and then the next thing would be to ensure you've changed the work off number on the planes page incrementing it up for each B - Axis rotation.

[CADCAM3D5AXIS]

Thanks For The feedback Chris.

Looking Forward to the update.

PS   pass the word along to the post team and tell them Thanks For All That  they Do .

It is Much Appreciated .

[Leigh @ Kodiak]

I'm using the same work offset for the whole program. 

 

What is causing my problem is that I am using 5 different block deletes to control which component is being run. If the first operation for a particular tool gets skipped due to block delete, I need the next operation that is not "block deleted" to have the WCS in that particular operation's first move.

 

Basically, I need a WCS output on the first move of each and every operation. Yes, I could acomplish this by forcing toolchange on every op, but as I stated, that is going to add  a lot of unnecessary motion.

[Mr. Wizzard]

what do you have set for "axis control" in your operations?

i set that and always get my rotation output. od thing is, i have to have it "off" on a drilling cycle to get it to post rotation.

and, dont mean to be too technical, but it's your t-plane that will give you rotation, not wcs. if they match, no rotation.

[Leigh @ Kodiak]

I am getting rotation output, what I am not getting is my Work offset on the first move of each operation (G54.1 P1 in my case)

 

Sorry if I was unclear about that.

[Sticky]

Hey Leigh, I know this isn't exactly what you want, but it's another way to make your situation work...

 

You could just have a different offset for each B rotation, and just set all the offsets in the control to the same values. And there are three ways you can do that, set all the offsets in the control by hand, manually enter G10's for each offset and their values using a MNP in the top of your program, or set your post to automatically calculate your offsets and enter the G10's in the header of your program (I do the latter).

[MIL-TFP-41]

in your PWCS section...

change this

 

        if workofs$ <> prv_workofs$ | (force_wcs & toolchng) | sof,

to this

 

        if workofs$ <> prv_workofs$ | force_wcs | sof,

[Leigh @ Kodiak]

 

in your PWCS section...

change this

        if workofs$ <> prv_workofs$ | (force_wcs & toolchng) | sof,

to this

        if workofs$ <> prv_workofs$ | force_wcs | sof,

That did it.

 

Thanks