HORIZONTAL POST AND JOB SETUP

[PBREMER]

Looking for help to setup job and to post

out toolpath for 3 axis w/ 4 axis indexable.

The Current problem I have is that when

I mill in front (tplane) the post handles it

just fine, when rotated to +/- 90deg, to pickup side holes, I expected 'G55' and 'G56"

for each of the positions, they never showed in the posted output.

If I start with the table indexed, then move to the front tplane, the output is all messed up and some operations never posted at all.

Does anyone have a specific way of setting up the jobs? is it necessary? and What type of post works good for this.

I am currently running all Horizontal MAZAKS.

and would like to hear from anyone with

Mastercam and Mazak experience...

All help is greatly appreciated.

P Bremer

Manufacturing Engineer

 

[Guest CNC Apps Guy 1]

It is not correct to assume that when you index that a new fixture offset will automatically be generated.

My usual programming procedure for horizontals is that I model the fixture (Tombstone - or whatever) program from the centerline of rotation as X0 and Z0, then Y0 is set as the top of the pallet and as each operation needs a different fixture offset I put that number in the operation. I have always done it this way and been quite successful at it.

If you want, I can post (in the ftp site here) a 630mm tombstone in the correct postition to get good output from MPFAN with no editing. There are even some simple drilling, contouring and facing operations in it too.

------------------

James Meyette

[PBREMER]

Thanks James for your reply.

I am new to programming using the 4th indexable axis, and all your information is greatly appreciated. From what you said above, my setup needs to change. I have been trying unsuccessfully to setup the part with the origin at one corner of the part.

Would you please post the 630MM tombstone file you mentioned above?

What is your procedure for rotating your TPLANE. How important is this... with this make or break a job?

One last thing. We have used verify alot and works well for 3 axis output. Will the tombstone file (with 4th indexable) work in verify as well.

Thanks in advance...

Sincerely

P Bremer

 

[Allan Brown]

Mpfan.pst or Mpmazakm.pst from the V8.1 install should automatically generate new WCS values for each face of your part if you leave the Work offset set to -1 (default).

For horizontal machines, set the following in you post:

vmc : 0 #0 = Horizontal Machine, 1 = Vertical Mill

rot_on_x : 2 #Default Rotary Axis Orientation, See ques. 164.

#0 = Off, 1 = About X, 2 = About Y, 3 = About Z

Also change the prefix for the rotary axes for example to 'B':

fmt B 11 cabs #C axis position

fmt B 14 cinc #C axis position

fmt b 4 indx_out #Index position

 

[PBREMER]

Thanks for all the help.

I am up and running now. The problem was

the way I set my part up. I was using the

0,0,0 corner in the center of my rough stock,

and not the way it was going to look like in the machine.

Backploting is looking good too, but the part doesn't rotate, the tool does. IS this correct? I have downloaded the ctour8.dll patch, that didn't help at all.

Can I please send my simple (small) file to

someone to see what I have got set wrong for my backplotting? (this is in reference to

a similar posting about 4 weeks ago)

ANy help is always appreciated

Philip

[Guest CNC Apps Guy 1]

Not changing tool planes will break it for sure. I mean you can program like you would a vertical (not taking in to consideration the centerline of rotation) BUT you'll have a bunch of edits and if you have to edit code, what's the point right?

Sooo, webby, where should I post the file?

------------------

James Meyette

[PBREMER]

If you want.. you can send the sample file directly to me as an attachment, using E-mail. Just click on my Mail Icon to get my address.

When I recieve it, what in particular should

i be looking for? I almost positive I have already been changing my tool planes. The posted output looks good.

Thanks for your response.

P Bremer

[Guest CNC Apps Guy 1]

You should be looking for how the tool planes are mapped. When you post this out using MPFAN, you’ll see the rotary axis indexing. When switching between toolplanes, I typically use “Normal” and pick a line that is normal to the direction I want z to be going into. Continue to select next until the axes are oriented correctly. The number of times you need to select next varies according to how you picked your normal line. Have fun.

. This has been the most reliable method for me so far.

------------------

James Meyette

[Webby]

>Sooo, webby, where should I post the file?

Upload to anon FTP at ftp.emastercam.com/incoming

Inform me of the file via email and I will move it to a location where others can download it, and post the link here.

[Guest CNC Apps Guy 1]

OK, she's in there. Check it out. It's nothing fancy but it shows the principles of Tool Plane machining.

Have fun.

------------------

James Meyette

[Webby]

Download James' File

[Guest CNC Apps Guy 1]

BTW, if anyone has any tips or tricks, please share with us. I just showed what has worked for me but I'm certainly game for seeing some new ideas.

------------------

James Meyette

[CycleTimeCharles]

James, for horizontals I make B0 the front plane not the top. I quess it depends on how your post is setup.

[Guest CNC Apps Guy 1]

I got used to doing it that way. The post will now take care of that so you can use the front and sides. The post basically re-maps your axes.

------------------

James Meyette

[Toby]

We use the cl of rotation for programming our Horizontals. It works very nice.

------------------

Toby Baughman

Magic Mfg

[Guest CNC Apps Guy 1]

I believe that programming from Center Line of Rotation is absolutely thhe best way to program horizontals. JMHO

------------------

James Meyette