G7 output in post

[Jim at Gentex]

This is a question about programming with a G7 toolplane tilt and having the correct orientation.

 

This is for a 5 axis drill program I'm having a problem with. The wcs, tplane, and cplanes are all correct in Mastercam, and the backplot looks good, but when I post it out I have a problem.

 

It's probably something in my post, but I'm not sure where to look to fix it.

 

What I want is this:

 

G7 L1=1 A5=0 B5=-46.5 C5=0

 

What my post is giving me is this:

 

G7 L1=1 A5=46.5 B5=0 C5=-90

 

Any ideas?

[Bruce Caulley]

Looks like the axis orientation is 90 degrees out. There are some switches for that I am sure. Sorry, don't have a seat to play any more.

 

Bruce

[john316]

.

 

Is this a new post you're working on or has it been giving you good code before now?

 

.

[Post dept]

Jim,

 

In some cases it is possible to perform a tool plane rotation such as your post is outputting, but it depends how the machine rotates your coordinate system. If both the A and C rotation happen about the original machine coordinate systems (ie rotate 46.5 degrees about x, then rotate this new tool plane 90 degrees about the ORIGINAL z), the resulting tool plane will be equivalent to the single B rotation. This is how the G7 command should work.

 

Some machines/controls don't allow this though and require the rotations be done in a specific order. In these cases typically a post will output the rotation about the z axis first (ie G7 L1=1 A5=0 B5=0 C5=-90) and then about the x/y axis (G7 L1=1 A5=46.5 B5=0 C5=0). I doubt this is the case for your machine, it should handle everything on one line.

 

Not sure that this will help out your posting problem, but may help you understand the logic behind why the post is spitting out what it is.

 

Chris

 

[ 02-21-2008, 10:54 AM: Message edited by: Chris McIntosh ]

[Jim at Gentex]

Thanks for the replies!

 

Good question john316.

The post was recently upgraded from an older version, so this is the first time I'm trying 5 axis drilling with the updated version.

 

Chris,

Thanks for the explanation, and yes, it does help in my understanding. The machine (DMU80T)is only 2 years old and it will do simultaneous rotations with a single G7 call.

 

As Bruce said, it seems as though the orientation is 90 degrees off. It's probably something fairly simple, I just don't know where to look in the post to change it.

[Post dept]

Jim,

 

I'm saying that the post needs to output the G7 in a very specific way to make sure your X,Y and Z coordinates are mapped correctly. The only difference between the two G7 commands you've listed is the direction of the X and Y axis, the Z axis should be pointing in the same direction in both cases. The post should be looking after rotating the coordinates to match the A, B and C output. Just because the plane you are cutting on in mastercam is a 46.5 degree rotation about the Y axis does not mean the code needs to be output as a rotation about Y.

 

If indeed you do need to change the post, chances are it's in the encrypted section of the post. You will most likely need to contact your reseller to make changes.

 

Chris