5 Axis 3D Curve Controlling B and C Axis (Head Head)

[RandyD]

First off I am fairly new to Mastercam and creating 5 axis programs, been creating 3 axis programs for years now, but now I have taken over the part of creating 5 axis programs and I am struggling with 3 main problems (previous programmer had the same issues).  We have been told/worked with our distributor that this is just the way it is and nothing there is we can do about these issues other than manually editing the g-code.  Where I work we have 2 5 axis machines both head head type with B and C axis on the Z axis and using TCP to run the same programs on both machines, both machines have 270 degrees +/- of rotation on the C axis. We mostly trim out thermoformed production parts using CNC vacuum nests.

1.  B and C axis randomly inverting themselves in a program say from B90 C90 to B-90 C-90.  Basically the B and C axis will be trimming the feature and then the next feature 2 inches over in the same plane it will completely invert B and C.  Currently having to manually go through the g-code and correct any "inversions."  Of course Mastercam/Post Processor? doesn't pull the head out of the part when it randomly inverts B and C.  I have noticed when previewing the program in Mastercam it does occasionally show B and C inverting, but other times it does not, so I'm guessing the Post Processor is causing some of the issues?  One particularly aggravating part I had a bunch of holes and slots all in one plane on the front of a part, it inverted B and C a total of 4 times!  WHY?  Grrrr!  For what it is worth Mastercam only showed one inversion in the simulation, where'd the other 3 come from?

2.  Controlling the unwind of the B and C axis as well as very unnecessary unwinds.  WHY! WHY! WHY! WHY!  If Mastercam/Postprocessor?? would just wind the head up to start with it wouldn't need to unwind.  We have an easy 360 degrees of rotation on the machine if it would just wind it up to say -180 and as it goes around the part unwind to +180.  Sometimes it will have 2-3 unwinds in a program just to make it 360 degrees around a part!
Next problem is the unnecessary unwinds, I declare it likes to put unwinds in the program just to aggravate me at times!  The program will be trimming around at say C90 and it decides it needs to unwind to finish the last turn (another 90 degrees to C180).  HELLO the machine has another 180 degrees it can rotate on C why the bleep does it think it needs to unwind??  Or even worse it will finish the last turn with just a straight X or Y left to go and it decides it needs to unwind!  WHY?!  It is a freaking straight cut!

3.  Finally third being able to control B and C axis orientation in a cut  Basically we have several parts where we need to the BC head to trim in a certain orientation so the head has clearance (say C-90 +/- 60 degrees), I declare in every incident where I have had this Mastercam/Postprocessor has put the orientation completely opposite of what it needs to be and I have had to spend hours manually changing the g-code.  I have tried everything I know how to do to get the g-code I need from changing the machines definitions and postprocessor that the machine only has -180 to 0 degrees of rotation on C.  Even with that it will still post the code out as +90 or -270

Any help on these issues would be greatly appreciated!  Like I said our distributor just told us that is the way it is, in which case why even pay for this "steaming heap pile" when I end up having to manually program it anyway?

[gcode]

Your dealer is wrong

A properly configured post and good programming techniques 

can produce efficient edit free code.

[So not a Guru]

gcode is absolutely correct, a properly configured post will generate perfect code, that requires absolutely no editing. Are you using the Generic 5X post that comes with Mastercam? I would highly recommend that you purchase a post from Postability or In House Solutions.

Your dealer is doing you a great disservice, if they in fact are telling you that nothing can be done. Are you talking about a Mastercam reseller, or the manufacturer of the router itself?

[RandyD]

We are talking with the Mastercam reseller, and we are using a post processor that as far as I know was created for us by our dealer.

[huskermcdoogle]

1 hour ago, RandyD said:

We are talking with the Mastercam reseller, and we are using a post processor that as far as I know was created for us by our dealer.

Sounds like your dealers post developer needs to go get some 5ax training, or someone needs to get remedial customer service training.

If you are able, you can make the generic post function well with a head/head and TCP no problem.  All of the issues you have described should be non-issues.

Here is what I would do.  Let's see where your 5ax knowledge level is at, and see if we can't diagnose and cure a few other things quickly.

1) Do you understand the purpose of the Misc Ints at the operation level, and how they affect the 5ax code output? Specifically Ints 4, 5, and 10. 

2) Are you contouring through an axis singularity when these flips occur?  (tool axis parallel to primary rotary), if so, you should tip your parts out of plane a little bit, and this should cure that problem.  Parts square to the machine axes aren't always a good thing in the full 5ax contouring world.  If this is the case than your dealer is pretty much telling you something close to the truth.

Question about the post:

2) Is your post based on the Generic 5ax post and are the misc ints mentioned above or a similar construct even used in your post?

3) If it is based on the generic, search in the post and report back and let us know if bias_null is set to 1 or 0?  This well greatly effect control over windup behavior between operations.

 

If none of the above questions ring a bell, then you will likely be best suited to go purchase a post from a reputable post developer.  They can help you massage your operations to use the post they provide properly, and get you edit free code with ease.

 

What brand and model of machines do you have?

 

Good luck,

Husker

[RandyD]

I think I understand some of the misc ints, like I said still learning!  4 Try to start C negative, I've tried both ways on this one with no change (set to false), 5 Clamp Rotary Axii I have not done anything with (set to false); and 10 is max feed for pivot (set to 800)?

For the post it says it is the generic 5 axis mill post and then under the rev log it says Axsys set it up.  I searched for bias_null and nothing was found.

We have a CMS PK and Athena both with OSAI controls

[gcode]

B controls the C

There should be a switch to force B + or -

This will drive your C giving you control over if and when rewind happen.

The basic principle of 5 axis programming is that every vector has 2 solutions

Forcing B + or - allows you to choose the starting vector that minimizes or eliminates rewinds

The wrinkle is that a vertical vector has infinite solutions, which is why your C sometimes goes nuts 

as B passes through 0

It sounds like you are running a lightly modified mpgen post

There are better solutions availabe

 

 

Edited September 24, 2017 by gcode

[huskermcdoogle]

We have two CMS machines here.  Both with Fanuc controls.  Can't speak for needs of the Osai controls much.  But I would imagine the kinematic arrangements are pretty similar to or the same as the antares and ares machines currently in production.  Maybe you could post a sample file?  We could then see what you have done with your ops and make some suggestions?

 

[RandyD]

I've played with this further, one thing I did find out was that the machine definitions limits where not set for the B and C axis, so I have now set them to the min/max limits, this however did not make any difference.  I have attached 2 files, just a "simple" around trim of a rectangle part with 1" radius, notice how the first part starts at C90 and goes up to C270 and then unwinds, while the second part also starts at C90 and goes around to C-90 and then unwinds, which it shouldn't be doing since the machine can go to -270.

For the first program Mastercam in the preview shows C-90 and rotation around to C270, which is actually what I want, it just doesn't post that way.  The second program Mastercam shows C starting at -90 and rotating to -450 (um the machine can only do -270???).

test.nc

test2.nc

[Colin Gilchrist]

Hi Randy,

First, you must determine if you are using a Post that is based on the Generic Fanuc 5X Mill Post.

If you are, then none of the "post setup" is done through the Machine Definition. All of the setup of this Post (Including the Rotary Travel Limits) is done by editing numeric variables inside the PST file itself. Changing the settings inside the Machine Definition has no effect on the Generic Fanuc 5X Mill Post.

 

 

 

[RandyD]

The post says it is a Generic Mill 5 Axis mill posts and under the edit notes it says it was setup for our machines by the dealer (axsys and barefoot CNC).  Not sure we are going to get much help form Axsys at least from what I've been told by our engineer who is in charge of all of this he has already contacted/worked them and to my understanding they told him it is what it is and that is just the way it is with the BC and axis.

Thanks for all the help so far, sounds like we need some help with the post, which is what I rather figured.

[gcode]

Randy, what version of Mastercam are you running

I want to put together a demo file and want to be sure were both on the same page

I have X9 MC2017 and 18 installed on my home machine

[horry]

i have a similar problem i try to solve for a long time. i want to cut only the small corner radii with no or minimum unwind moves. in those pockets. try the +- solution without sucess. 

its a special 5axis post from MPPOSTABILITY

 

unwind again.mcam

[crazy^millman]

4 hours ago, horry said:

i have a similar problem i try to solve for a long time. i want to cut only the small corner radii with no or minimum unwind moves. in those pockets. try the +- solution without sucess. 

its a special 5axis post from MPPOSTABILITY

 

unwind again.mcam

You have no toolpaths in the file. We need a file to follow along with you.

[horry]

acctually i finally figuered it out. i used to control the axis by just a point rather a chain. parallel 5 axis seems to work best.