McX6 Rotary 4-axis roughing

[Doug Overkill]

I am using MCam X6 and have a part programmed using the rotary 4 axis tool path. It seems to be working as expected but I have 2 issues. One is an annoyance and is probably a post processor issue and that is all of the A values get posted opposite from what they should be. Meaning the A+values should be A-values and vice versus. The graphics represent what I want to happen and if I do a cut and paste in my NC code from A into A- and then A-- into A I get a program that runs and looks just like the verify and is what I want to happen. I have played with the climb vs conventional cut parameters as well as most everything I could find within the toolpath settings with no luck. I have played with a bunch of parameters with in the machine definition and again no luck. I was unable to get any change in the A +/- sign. Any ideas? This is a little less critical to me as I have a work around all be it an annoying one.

 

The more critical issue I am having with the toolpath is the ability to rough and finish. Ideally i would like to define a max tool depth and have the tool step down in Z at that increment and then perform a finish pass at the final Z height. Then step over in X and do each roughing layer until a final z depth is reached. Each time only moving over in X once the part has been roughed and finished. The only work around I have found is to break my toolpath into zones and create an operation the roughs from X0 to X-.25 while leaving an amount on all surfaces. Then finish that zone. Then rough a zone x-.25 thru x-.50 and then finish that zone.

 

I have attached a part that I hope shows what I have got to work, but is not what I want to do.

 

Thoughts?

BENT-ROD.MCX-6

[JayM]

I would try a Parallel cuts multiaxis toolpath. That should get you what you want.

[djstedman]

So far as the inverted signs on the A moves are concerned, If the graphics are truly right on screen ie. part orientation matches part orientation in the machine..

 

Then this is most likely caused by one of two things, either the post is setup with the A axis positive direction going the wrong direction, or a parameter in the machine is set to make the rotary rotate the wrong direction..

[CJep]

Depending on the post you started with you should be able to open the properties for the A rotary axis in the machine definition.

If you are using a post that you have updated from a version of Mcam prior to version 10 then that post will not have the machine / control def functionality of the newer format posts.

The MpMaster mill post is solid and can be downloaded from the forum and has the functionality.

 

To change the direction of the A axis open the machine def -

Right click on the VMC A axis in the machine configuration -

Open the properties of the A axis -

Change the direction by changing the rotation to CW or CCW -

 

You can do this as a local change in the part file by using the edit command in the machine group properties, once you have the rotary going the correct direction make the global change in the settings dropdown.

[Doug Overkill]

I was wondering if the multiaxis parallel cuts would do what I want. I will need to spend some time looking into that as I have never used it. Thanks for the suggestion.

 

I was thinking the issue with A axis direction may be in Machine parameter control. Is there a "standard" for A axis negative direction? Should A axis "ALWAYS" be negative for CCW when looking at the face, or is this a variable across platforms?

 

Cjep - I have done the cw/ccw changes but it did not effect my final output. My issue may be because the post was once from V9. (V9 is still my favorite!)

[CJep]

My issue may be because the post was once from V9. (V9 is still my favorite!)

 

That post is not going to respond to the machine/control def files,....

 

If you have the ability to use multiaxis toolpaths, here is a sample toolpath using 5axis flow,..

 

Edit: use this file instead, I changed the cut type to spiral and shortened the pattern surface

[Doug Overkill]

CJep-

I looked at both files you sent over. The second one looks similar to where I am at now with the rotary 4-axis. When i try to turn on the ROUGHING, DEPTH CUTS I get an error that says "Select Tool Pattern Surface". It doesn't matter what surface I choose, it gags out. Sometimes it completes toolpath but nothing like what I am after, usually just one surface is being cut. I tried to change any other parameter and got same question.I appreciate your help on this.

[CJep]

Doug you have to select the pattern surface, that's whats driving the toolpath motion, it's on level #10

[Doug Overkill]

Hi Cjep - So you have what I had using rotary 4-axis, Thought I like the flow path better. This 3rd version you sent over does an entire spiral pass along the X axis from X0 to X-1.17 leaving 0.12 on part. Then it does another pass from x0 to x-1.17 leaving 0.06 on part and then a final pass finishing the part. THIS IS NOT WHAT I AM AFTER.

 

What I want to happen is to rough at each X location then finish. Then do the sep over. So...

At X0 cut a single spiral or loop of the rotary leaving the 0.120 extra. Then still at x0 do another loop leaving only 0.06. Then a final pass still at x0 finishing the part at this point.

THEN step over in x by the increment (0.025 in this program) and now do a +.120 pass at x-.025, then +.060 pass still at x-.025 then finish at x-.025.

THEN step over in x to X-.050 and cut a +.120 pass, then +.060 pass then finish pass. Then step over and repeat. By doing it this way the material self supports> If I do it the other way I can't acheive the finishes I am after because the x0 end is to flimsy.

 

Does this explain my intent better?

[CJep]

There are a number of ways to change up this toolpath, you can change the direction of the flow the same as changing a 3D flowline surface tpath. To do that open the flow parameters for the pattern surf in the cut param and you can change the cut direction. You can change the cut from spiral to one way. You can change the roughing param to cut by contour instead of depth.

 

This is a sample tpath written to your geom, change it up to what ever works for your situation.