MultiCam 3000 Post Problem Fusion 360 Z axis is offset

[PeteMwms]

 I am new to both MultiCam and Fusion.  I have already discovered the feed rate problem but I'm having an issue where  the Multicam is not seeing the correct  z origin or it is offsetting the tool path in the wrong  direction. 

I am following the MultiCam 3000 Instructions and setting tool height on the top of the item to be milled.  All of the tools are zeroed  in the correct fashion. 

I also set the max depth at the surface of the machine. 

The indications are that the post processor adds the thickness of the part to the top of the tool height  and uses that as a start point

The hand held control shows Z= 0.000 when the tool is on top of the part.   the G code shows -2.00"  for a 2" part top which is actually 2" above the top of the part.

The part origin is Z up and the X-Y plane on the machine surface.

Any help would be appreciated.

[mcarver · Accepted solution]

pmgroupsg

This sounds like a simple miss-understanding on the setup of the job in the software.  If I understand you correctly you are setting the wcs on the table in the cam software.  So it is thinking that the tool needs to be at a height of -2 when the tool is at the top of the part.  Where you are setting the zero in your machine to the top of the part.  So when the code is posted a value of -2 is expected to be the top of the part where it is zero in your machine.

All you need to do to fix this is move the wcs in Fusion to the top of the part.  This should then match your machine and fix your issue.

[Laurens-3DTechDraw]

To me it feels like the machine's Z-axis is inverted.

[PeteMwms]

 Moving the origin to the top of the part did in fact fix my problem.  It took me a little time to actually do it and test it on the machine. 

It seems that when I use the auto bit  sensor to set the workpiece height it resets Z -0  to the plane at the top of the material  There is a second setting of the max depth the cutters can go and that is normally set at the machine surface.  It seems that this is more of a safety setting to protect the spoil board,  or if this was a CNC Mill the top of the work holding surface. 

[ICanSpinIt]

Have you dealt with the retracts on drilling? The retract is opposite on this machine. Multicam said “its a cnc not a milling machine”  ! 

[PeteMwms]

I have had an issue with rapid retract drilling with the Standard Post
processor actually moving the spindle to the next point before fully
retracting. My work around is to always use a pecking type drill operation
when using drill bits. this has worked for me.

Also I had an issue with the fee speeds because of a mismatch on how my
machine was set up. Its controller (2008) version would translate the feeds
to IPS even if written in IPM. I had a friend write a custom post to solve
this issue.

Pmgroupsg

[ICanSpinIt]

Lol yes! I found the ips issue today as well. I now know how fast you can cut HDPE, ****ty edge but super fast! Ill be trying to figure out the post processor out all week for that one! 

[PeteMwms]

I just divide the standard feeds by 60 so most plastics become 2-3 for
1/4" coated bits single flute Whiteside RU2074A o-Flute works 1600 rpm
Rough cut to about 0.010" to leave a skin to clean ( we Use a 20HP vacuum
system to hold material

The real speed limit is how well you can hold the part down. I also use
carpet tape to assist when doing small parts especially those that can be
sucked up by the dust collector.

For accurate sizing you need to take a finish cut on the critical edge as
most soft plastics move with the cutter and rebound.