Force a T\C Plane in posted code

[DavidB]

I have a part in a Vertical 5-axis machineing centre that is running in the Y-axis on it's fixture. Here is a pic of the standard TOP view.

 

 

This part is out of the machines Y-axis limits so when I machine it I want the C axis to rotate 90° so that the part is now running along the X-axis.

 

So I rotate my TOP TC Plane 90° and create my toolpath using this rotated T/C Plane.

But the posted code is still at C0 and not C90° how do I get this rotated TOP plane to out put as the part running in the X-axis?

 

Here is the part in the rotated Top plane

 

 

The machining is done in the Y-axis and at C0?

[GI George]

I would go to top view, rotate Gview 90 deg., name and save current view. go into your tool path, planes set your WCS to top and then your T and C plane set to the 90 deg that you made should work. May be someone else has a better way?

[DavidB]

I have that but it still outputs using the standard top T/C plane.

 

[GI George]

Dumb question, you have the correct post selected?

[DavidB]

Yes

[DavidB]

I think its in my post.

Could someone please email me the Generic Fanuc 5X Mill post for X4 so I can cross referance?

 

Thanks Dave

[Mr. Wizzard]

It just doesn't look right. Shouldn't the X-axis be running through the length of the part now, not the Y-axis?

That's what you're shooting for, right?

[DavidB]

In the created Tool plane yes the X-axis is the long axis of the part.

The post should use the toolpane to create the rotary moves 3+2.

But its not for a rotated Top plane strange.

 

If I use a 4-axis post it works but not a 5-axis post.

 

I have to get this job running tonight. So what I have done is rotate the WCS 90°, this gives correct X,Y and Z moves with no rotary posisitions which I will just add in for now.

 

I have sent the file into posts at CNC. See what they say.

 

Cheers Dave

[gcode]

quote:

---

Could someone please email me the Generic Fanuc 5X Mill post

---

there should be a copy at

C:mcamxmillpostsGeneric Fanuc 5X Mill.pst

 

have you tried forcing the rotatary output with

mi4 and mi5??

[DavidB]

gcode the Generic Fanuc 5X Mill post is not in my web install of X4.

 

quote:

---

have you tried forcing the rotatary output with

mi4 and mi5??

---

[gcode]

I don't know how your machine is configured

so I don't know which is primary and secondary,

but you can use the

Intial Primary and Initial Secondary to force

rotations at the start of an operation.

Try puting 90 in Initial Primary and post the operation..

I emailed you a copy of Gen Fan 5x.. I forgot

to change the pst extension and some AV softwares

quanartine files with a pst extension... so if your AV software gets all hot and bothered with my email that's why..

 

 

mi4 and mi 5 from the post notes

 

# mi4 - Start initial primary rotary axis bias

# +/-999 represents start as close to limit as possible

# 0 represents calculate without using bias

# Any other value represents an angle in degrees to attempt

# to position near.

# -999 = Low, 0 = Off/Default, 999 = Hi, Value = Angle bias

#

# mi5 - Start initial secondary rotary axis bias

# +/-999 represents start as close to limit as possible

# 0 represents calculate without using bias

# Any other value represents an angle in degrees to attempt

# to position near.

# -999 = Low, 0 = Off/Default, 999 = Hi, Value = Angle bias

[DavidB]

Thanks G yes I can not recieve .pst files.

Please rename to .txt or .zip and resend.

 

Thanks Dave

[Alvaro Gil - Cimquest-inc.com]

You will not be able to post that with the 5x post. do it with the 4x. There is just no functionality in the 5x post, to rotate just the top plane and have it post out.

 

Post gurus, please correct me if I am wrong, I have had this request several times and have not been able to find a better solution.

[DavidB]

Alvaro

A rotated top plane does work with a 4-axis post but a rotated Top plane with a 5-axis post does not seem to work. Strange shouldn't the post use the T plane for 3+2 programming.

 

This is the first time I have run into this problem. Not to often I need to rotate the top plane but on this occasion I have too.

 

Gcode the Mi-4 puts a 180 degree move in and all the X,Y co-ordinates in the posted code are still using the standard Top planes. Backplot how ever shows the correct co-ordinates. So it's definatly a post issue.

 

I'll be intersted to see what post devolopment have to say about this one.

 

Cheers Dave

[gcode]

What happens if you use your rotated top plane in all three fields WCS, Tool Plane and Comp Plane??

New copy of post file on the way

[DavidB]

quote:

---

What happens if you use your rotated top plane in all three fields WCS, Tool Plane and Comp Plane??

---

It outputs correct co-ordinates just no rotary moves.

This is what I have done and edited the code to get the job out the door.

 

Cheers Dave

[Alvaro Gil - Cimquest-inc.com]

As far as I can tell, the 5x post does not have the functionality to position the xy plane via the WCS->C/T plane comparison that the 4x posts do. I have toyed around with the Misc values for hours, trying to get the initial angle to post out, but to no avail.

 

This is something I would LOVE to get squared away, if someone has a good option, other than posting it out on a 4x post, then I would love to know! I believe we are going to need a post mod to get this to work.

[Alvaro Gil - Cimquest-inc.com]

Dave,

 

I have used the same method. With mpgen5x, I don't think there is any other way. You can insert a manual entry before and after the toolpath to get it to output at least almost edit free. I will usually throw in a M00(check code before running first time) in case I forget months down the road..

[Joe788]

Dave, just curious, is this a Variaxis 500?

[dolphin1]

is there a setting to allow twist instead of readressing arcs in the post. that is what you need to get the 3+2 to work.

[Guest CNC Apps Guy 1]

CAMplete does this with a couple mouseclicks.

 

Have you tried doing swarf instead of contour?