Axis sub - cutting windows in cylinder OD

[nbet]

Please find the X2 file on the MasterCAM FTP at ftp://www.mastercam-cadcam.com/Mastercam_...5-105_OP070.zip

But I see that the link doesn't exactly work.

 

I have chained the contours and the tool paths look reasonable. But when I backplot or verify, I find that the cutter is leaving some material all around the inside of the cutouts. I also used the Compare to Model after the true solid verify and it did show excess material still left on the contour.

 

If you look at the backplot you see that the cutter is running inside the contour instead of on it. I think this must have something to do with the unwrapping, axis substitution, cylinder diameter, etc.

Remember when using backplot to turn on Simulate Axis Substitution and turn off Simulate Rotary Axis!

 

Any help, guesses, or comments are welcome.

Thanks

Noah

[crazy^millman]

Did you program it using Axis sub?? Did you program to using 5 axis curve? Did you program it using 5 axis swarf? Did you program it using Roll-Die?? Sorry did not look at the file, but these would be my choices for what you are talking about.

 

Did you try cutting a .002 deep pocket on the part to see what it looks like?

 

Thank you for zipping that file. You link worked just need to put Mastercam in for user and swiss for password.

 

Welcome to the forum.

[crazy^millman]

Ok looked at your file the walls not being normal to the center are what is causing you the big problem. This is where a 5 axis toolpath in 4 axis output would be very helpful. The big question is do you have Level 3 with 5 axis capability??? You did a lot of things right here, just the part will not play nice with axis sub the way you have now.

 

I did a toolpath for you using 5 axis curve. I also use entry to eliminate the need for a hole to start the toolpath like you were using.

 

 

Oh one other thing you can use your solid from the previous op as a solid for your verification. If you have X3 the 5 axis verify is free now for that version again going off the idea that you have the full capabilities of Mastercam.

 

HTH

[nbet]

Thanks Crazy,

but I don't understand what you mean by, "walls not being normal to the center". I did check that out prior to programming and found that the windows are radial 'pie slices' that are subtracted from the cylinder. So, everything should be radially symmetric.

 

But you're hitting on something I noticed, that the tool is not cutting parallel to the window walls. Can you explain why?

 

Thanks for messing with this, I really want to understand. I did not find your file using 5-axis curve. What it is named? I do have full Level 3 capability so I'll check out your file if I can get it.

 

Noah

[nbet]

Ok,

 

I found your file, ftp://www.mastercam-cadcam.com/Mastercam_...5-105_OP070.zip

 

It does look correct in that it follows the contour. There doesn't seem to be any reason that I couldn't use this approach. But I still have the question about "walls not being normal to the center"...

[crazy^millman]

Walls are normal to the center sorry for the confusion. The tool's center line need to be normal to the center and the walls would then at the index angle really need to be off center line to be cut with the endmill using your current approach. The axis sub has a hard time cutting some stuff on center line then others off center line. You can do it, but requires some tweaking to your chain to get it to cut correctly.

 

HTH

[nbet]

I think I understand about the tool needing to be on centerline. That sucks, is there a workaround?

 

The problem now is that when I post your method, I don't get B-axis moves, it's all X,Y,Z moves. But when I post my axis sub toolpaths I get the correct output which is B,Y,Z moves. Do you know why?

[John Summers]

ROLLDIE.DLL was designed to cut walls that are radial from the centerline. The reason that axis substitution does not give you radial walls is that the rotation angle is figured from the cutter center. ROLLDIE figures the rotation from the drive geometry (the wall). CURVE5AXIS also figures the angle from the drive geometry, but needs a surface, in this case a cylinder, from which it finds a normal, and you have to work in 3d. ROLLDIE can work from either 3d models or unrolled geometry.

[nbet]

Thanks for the ROLLDIE.DLL advice. It looks good in verification but, again, the output is all X,Y,Z moves instead of B,Y,Z moves.

 

I now have three tool paths in my file; 2D Contour using axis sub, 5-axis contour with 4-axis output, and the Rolldie operation. The only one that outputs moves using the B-axis is the first method using axis substitution.

 

Please see my X2 file at ftp://www.mastercam-cadcam.com/Mastercam_...5-105_OP070.zip

[crazy^millman]

Ok what post are you using? How do you have your machine def set-up for that post??? I have seen few verticals that have the indexer along the Y axis so need to make sure you have your axis set-up right in the machine definition.

 

HTH

[nbet]

This post is for an horizontal mill. The B-axis rotates about my Y-axis. The machine defs are correct as is the post.

 

I have added my post and machine definition and control files at ftp://www.mastercam-cadcam.com/Mastercam_...5-105_OP070.zip

 

I assumed that since the axis-sub operation posted correctly using my files that the 5-axis and rolldie would as well. Maybe that's not the case.

[crazy^millman]

Ok well you have set-up as a vertical machine. Who did the changes to the Machine definition that go against what Mastercam supports for this on Horizontal machines??? Mastercam requires you to Make front A0 not top A0 and your current set-up is probably what is causing you the problems you are seeing with other toolpaths and not Axis sub. Try moving everything to front then repost and see what happens. When I say everything I mean the c-planes and T-planes, not the WCS. If you feel you can only program a Horizontal this way then you need to use a vertical machine definition and then just modify it to output the code the way you want.

 

In the next 5 years Mastercam should have their machine simulation worked out for these machines and in 5 years you will not see it backplot it correct.(5 years is probably more like 10 using the current MMT development as a bases for that time line estimate)

 

HTH

[nbet]

Interesting! Your suggestion to change T/C planes did the trick for the ROLLDIE operation output. Thanks.

 

I didn't expect this sort of problem. I am using an installation/configuration that I didn't set up. Looks like I need to do some investigation of the reason for the strange machine config file.

[crazy^millman]

Ok but did you move the part as well and not just the t/c plane?? If so yes it may have output, but would be the wrong output if you did not move your model and geometry. Look in the probing question the picture by Jim in there represents what the part should like when you look at in Mastercam in ISO view. WCS top, C/Tplane front for A0 and away you go.

 

HTH

[Jayson Kramer]

Nbet, linking to the FTP directly to a file does not work. as there are user name and passwords.