5-Axis Drill Bug / Warning (X5, X7)

[PMDc]

Has anyone else seen this?

 

It appears to be a bug going back to at least X5 and still present in X7.

 

We are running 4-axis horizontal Makino A61's. All paths are set with WCS to TOP and any Tool/Const Planes set as needed. i.e. Front, Left Side, Custom, etc.

 

In the 5-Axis Drill operation parameters under the Tool Axis Control there is a Rotary Axis setting for X, Y, or Z. Mastercam Help says this setting is based on WCS so since our B-axis (rotary) is about the Z-axis that is what is selected and Mastercam says it's valid. However, the code is wrong and back plot reflects it.

 

In order to get the correct code this must be set to Y-axis. However, when you reopen the file it goes dirty because Mastercam says the path is not valid with the Machine Definition.

 

Is no one using 5-Axis Drill? Or are we doing something wrong? I have tested this on the supplied Mastercam MD/CD's as well as the custom ones we use. No change.

 

We have tried all logical WCS, TP, CP combinations with incorrect code results.

 

Thanks,

-Pat

[Joe788]

Interesting. Is your post set up for TOP>TOP as B0, or are you using TOP>FRONT for B0?

[crazy^millman]

Pat are you making sure to keep your levels on that have the lines defining the holes? I only teach people to 5 axis drill using Hole Axis with points and lines to the bottom of the hole. Anything else can be extra work not needed.

 

HTH

[Colin Gilchrist]

This is most likely just a Machine Definition issue, and not a problem with the toolpath itself.

 

When you first open a Mastercam file, there is logic that checks the Machine Definition to see if the machine has valid rotary axes for the toolpaths you've programmed. I believe that there are some problems with Horizontal machine definitions, and how the toolpath settings not end up matching the Machine Definition, because it doesn't take the Toolplanes into account, only the WCS. So Mastercam looks at the MD, and sees that the rotary axis doesn't match the rotary that is selected in the toolpath.

 

The way that I typically get around this is to edit my Machine Definitions and make sure that I've got 3 rotary axes, A, B, and C. Each one configured to rotate around X, Y, and Z. In addition to adding the rotaries, you must edit the Axis Combination, so that the Axis Combination contains all three rotaries.

 

What this gives you is a Machine Definition file that is capable of cutting any possible toolpath that you can generate in Mastercam, and won't generate that error when you open the file or do a "replace" on the Machine Definition file.

 

The only caveat is that you should make sure the post is configured to not read the Machine Definition to set the rotary axis settings. If the post is a 4 Axis post, there is logic to read the MD settings to configure the rotary. If it detects more than 1 rotary axis, the post will generate an error. The way to get around this is to disable the switch that lets the post read the MD, then configuring the rotary settings inside the post itself.

[PMDc]

Thanks for the responses.

 

Joe - We use Top - Front for B0

 

Crazy - Yes all the levels are on, I turned them off for the screenshot.

 

Colin - It appears that my assumption was correct in that this is truly a bug if your approach "fixes" or more accurately "works around" the issue. If I have to lie about the machine in order to get Mastercam to not error then turn around and have my post ignore the lies.... that's a bug.

 

Thanks for the input! Helps alot!

[Colin Gilchrist]

What we consider a bug, others might consider a feature. I wish you good luck in getting it addressed. You should send the bug into QC and make sure you get a bug number.

[gcode]

Open your machine definition and add a 4 head aggregate to the end of your spindle

This will have zero effect on regular tool paths, but will trick a 4 axis machine definition

into running 5 axis tool paths

[PMDc]

Gcode,

 

This was the best work around for me. I still put this in my book as a bug or actually a parameter that shouldn't exist. If the operation is looking at machine kinematics then the rotary axis should only be needed for clarity for a 5-axis machine and even that is questionable, unless the Help file is wrong in saying the axis selection is about WCS when it actually is about the Tool Plane.

 

Thanks again for the post, This will at least stop the errors from coming up.

 

-Pat