Toolpath transform rotate

[bobbyjack]

Hi there,

I seem to be having a great deal of problems with trying to rotate operations for a horizontal part about the top view (Z world) 1 step 180 deg. First of all it didn't want to post saying only single axis movement was allowed. I then switched to rotate around origin instead of a point and at least then it would post but the numbers I'm getting aren't right at rotation. Mastercam seems to do OK until I hit a rotation and then I start getting minus Z values for clears and bad signs for either X or Y. Any suggesstions would be great.

[Harryman]

Check the rotation view on the Rotate tab under Transform Operation Parameters.

 

[bobbyjack]

I'm rotating in view 1

[robk]

quote:

---

Check the rotation view on the Rotate tab under Transform Operation Parameters.

---

+1 Harry

 

Just make sure you have the correct view assigned.

 

Rob

[robk]

quote:

---

I'm rotating in view 1

---

Is your geometry in the same view?

 

Rob

[bobbyjack]

I think the problem lies in that I,m actually doing a double rotation (rotating around Z for the transform and then around Y on the machine) I don't know if Mastercam will do this. The tech guys have looked at it but I don't think they understood what I was trying to do because true they got rid of the errors but the numbers are still wrong.

[cadcam]

what tplan is the program in?

[bobbyjack]

Yes, the geometry is in the same view. We always try to machine in the top view for B 0.0

[bobbyjack]

The toolplane is a copy of top named G54.1 P1 with a work offset of 1 (P1)

[robk]

I have tried to re-create your problem with a simple program I've made, but I can't. Double check all your paramaters. Pay attention to all your planes... Post the file on the FTP site if possible... I'm sure someone will help you (I don't have access).

Good Luck.

 

Rob

[mayday]

horz machine right??

 

do you have your geo file in same pos as on your machine. rotate on center of axis? I do this alot work from front plane, top plane will mess you up big time. rotate about y axis not z. see if that helps

[Harryman]

Are you trying to rotate a rotary axis on a horizontal mill?

 

If so try rotating around View 5, using Cplane method.

 

[ 09-17-2003, 03:03 PM: Message edited by: Harryman ]

[bobbyjack]

Here the thing, what I'm trying to do is take one part in the top half of a chick vise, rotate it 180 and put it in the bottom half of the vise and machine two parts at one time, I can't just move it down to the bottom half because of clearance issues. I'm not trying to move it to a different face of the tomb. It needs to be machined at 0.0,90.0,270,35 and -35 deg rotations. Hope this helps clear things up.

[mayday]

you try rotating the geometry copy/regen? instead of the toolpath or do you want each tool to cut all parts as it comes out. if I understand you correctly you are making the same part in differrent positions and orientations

[john316]

I've tried doing the toolpath transform rotate with multiple cplanes for 4th-axis rotation and Mcam went wacko.

The most reliable way i've found to do what I think you're trying to do is to rotate copy the geometry and reset your cplanes to the new rotations. This takes a little bit longer but the toolpath is reliable.

 

+1 MayDay

[bobbyjack]

I would like each tool to work on both parts.

 

Thanks for all the replies guys it really looks like I need to copy the geo and go from there

[mayday]

maybe this thread sounded more confusing than it is. when transforming a complete prg you get a lot of tool changes. take each opp and transform them individualy and resort the transforms and just post the transforms.it works better. get one to work first. watch all cplane tplane options

[Ron Branch @ 5th Axis]

Yes Bobby Jack this goes back to people who only use the WCS to d othis i dont I always copy my part inforamtion into every rotation angle then label all of my operation for each tool that works on each angle take some more times but not had any problems doing it this way. You can easliy create a file that is your tombstone then everytime you bring a new part use that as a template t olocate parts on it will save you laot of time down the road.

 

Crazy Millman

 

May the Mastercam force be with you.

[P_Scott]

bobbyjack,

 

The Transform-Rotate toolpath operation will accomplish what you want it to do if you are simply taking the same toolpath and machining on another side of your fixture or part. In the Transform-Rotate parameters, Rotate tab there is a check button near the bottom that says "Rotation view" and a "View #..." button below that. If it says "view #1" that means the toolpath will be rotated using the Z-axis of the World or Top Cplane, arranging your rotated toolpath around a selected point and placing it in opposite quadrants of the same plane.

 

If you want to use the X-axis as your horizontal axis of rotation, the "View #... button should say "View #5" to utilize the Right Side Cplane, so you start with toolpath on the Top plane and end up with toolpath rotated to the Bottom plane at 180 deg. Using the Y-axis as your axis of rotation would require the "View #..." button to say "view #2", or Front view to rotate the toolpath around. This would give the same result as before except that the index angle would output a "B" instead of "A" angle. You can also Copy the Transform operation and Rotate the toolpath again for your different angles.

 

The rotary axis angle values are post-dependent. This means that Mastercam will do the calculations correctly but your post processor will need to be set-up or modified to output the code the way you want it. It may be a simple change of a switch or two, or it could mean more complex changes. Your Mastercam reseller should have a class which discusses these issues. I highly suggest getting instruction on Transforming toolpath and generating operations to output for Horizontal machining. It takes a little patience but is easily accomplished in Mastercam. Sorry for the long explanation but there seemed to be a lot of confusion in this thread and there are many variables to consider. HTH

 

[ 09-18-2003, 03:14 PM: Message edited by: Peter Scott ]