Finding the Angles of a Double Angled Face

[Jake L]

I'm looking for a button in Mastercam, I'm not sure whether or not it exists. If this button doesn't exist, then I'm looking for recommendations on easier ways to do this.

Here's a link to a sample Mastercam file, my math notes, and a couple helpful screenshots: Dropbox Link

What I'm trying to do is find the two angles that make up a "double angled face". I can do the math out to get the angles (see pic above), but this feels like a huge waste of time. Is there a button in MC that will do this for me? 

I understand how to use the dynamic transform and align surfaces, but in this case I need the actual number of degrees for each rotation. I also understand there will be more than one solution to the proposed question. I am looking for the angles when rotated around the Top plan Y axis, then rotated around the Top plane X axis.

If an "easy" button doesn't exist for this, can anyone recommend an easier way than what I showed? I'll probably end up making some kind of excel "calculator" for this situation.

Please let me know if anymore information is needed. Thanks in advance. MC2023

[So not a Guru]

Are you looking for bisect line?

create a line on each edge, select Line bisect from the wireframe dropdown, select the two lines you created then select the bisected line you want to keep.

[Jake L]

2 minutes ago, So not a Guru said:

Are you looking for bisect line?

Thanks for the reply. 
I have used bisect line in the past, but I don't think it would be useful in this situation. Unless I'm completely overlooking something, which is entirely possible.

[neurosis]

I don't know if this is what you're looking for

Read through that and see if it is.  

It's certainly not an easy button but it works to get the rotation if you're trying to mill (or drill) a compound angle and you're stuck on a vertical machine with only a one axis tilt table.

[Jake L]

8 minutes ago, neurosis said:

I don't know if this is what you're looking for

Read through that and see if it is.  

It's certainly not an easy button but it works to get the rotation if you're trying to mill (or drill) a compound angle and you're stuck on a vertical machine with only a one axis tilt table.

That is exactly what I was looking for, thank you!

 

I never thought about using hole axis to get the angles, but that does the trick on my actual part. That absolutely is an easy button compared to doing out the math.

 

As for the sample file, there was no holes in the solid model.

This idea is untested, but I think I could load in a 5 axis machine, create a surfacing op, and set the tool axis perpendicular to the angled face. Then if I post that operation it should give me the two rotation angles. 

[neurosis]

1 minute ago, Jake L said:

As for the sample file, there was no holes in the solid model.

You don't really need a hole axis.  Just use wireframe and create a line normal to a point, select the surface (solid face) and a point.  You can put the point anywhere and still figure everything out.

 

1 minute ago, Jake L said:

This idea is untested, but I think I could load in a 5 axis machine, create a surfacing op, and set the tool axis perpendicular to the angled face. Then if I post that operation it should give me the two rotation angles. 

I believe that you're right but I haven't tested that in mastercam.  I do that occasionally in TopSolid if I want to save some time.  Before we had T/S I had to figure out how to do this in MC without the math.  We were doing this a LOT and my math skills leave a lot to be desired.    

[Jake L]

1 minute ago, neurosis said:

You don't really need a hole axis.  Just use wireframe and create a line normal to a point, select the surface (solid face) and a point.  You can put the point anywhere and still figure everything out.

I swear it is baffling how many new things I learn on this forum, thank you.

 

2 minutes ago, neurosis said:

Before we had T/S I had to figure out how to do this in MC without the math.  We were doing this a LOT and my math skills leave a lot to be desired.    

We rarely do this, but knowing how is a very important tool in my toolbox for when we do need it. 

I love the math behind all this stuff. Not saying I want to do all this out by hand all the time, but little problems like this break up the repetitiveness nicely.

[RsH01]

Make a plane form solid face, program a simple toolpath like a drill, contour or face, set wcs to top and the tool and construction plane  to the newly created one and post, you will see the angles in the posted program, you can use a generic 5 axis post if your machine is not 5 axis.

[Colin Gilchrist]

19 hours ago, Jake L said:

I swear it is baffling how many new things I learn on this forum, thank you.

 

We rarely do this, but knowing how is a very important tool in my toolbox for when we do need it. 

I love the math behind all this stuff. Not saying I want to do all this out by hand all the time, but little problems like this break up the repetitiveness nicely.

If you love the math, Mastercam Post Processors use Vector and Matrix Math (Linear Algebra), to derive all the rotary angle output for 4-Axis and 5-Axis. If you look at the NCI Data (raw toolpath motion) from a 4-Axis or 5-Axis Program, there are no Rotary Angles output in the NCI Data. All angles are resolved inside the Post Processor, from "vector inputs". For a 4-Axis Program, the Tool Plane Z-Axis Vector, is compared to the WCS Z-Axis Vector, using the 'atan2' function. For Toolplane processing, this is done 'automatically' inside MP.DLL (the Post Engine), which then sets the internal Rotary Variable 'c$'. (No matter if you are outputting "A" or "B" or "C" for the Rotary, the internal variable is named 'c$'.)

If you want to learn about editing Mastercam Post Processors, check out the link in my signature...

[Jake L]

1 hour ago, Colin Gilchrist said:

If you love the math, Mastercam Post Processors use Vector and Matrix Math (Linear Algebra), to derive all the rotary angle output for 4-Axis and 5-Axis. If you look at the NCI Data (raw toolpath motion) from a 4-Axis or 5-Axis Program, there are no Rotary Angles output in the NCI Data. All angles are resolved inside the Post Processor, from "vector inputs". For a 4-Axis Program, the Tool Plane Z-Axis Vector, is compared to the WCS Z-Axis Vector, using the 'atan2' function. For Toolplane processing, this is done 'automatically' inside MP.DLL (the Post Engine), which then sets the internal Rotary Variable 'c$'. (No matter if you are outputting "A" or "B" or "C" for the Rotary, the internal variable is named 'c$'.)

If you want to learn about editing Mastercam Post Processors, check out the link in my signature...

I have dabbled in post editing, mostly just reordering, adding, or deleting certain codes. I've never gone into the math of it, mostly because I haven't needed to. Someday I'll have an excuse to dig into the math, and I'm sure it'll be frustrating and make no sense... I'll love it. 

Thanks for all this information!

[Colin Gilchrist]

You can learn about the math involved, from Gilbert Strang, at MIT, for free, here:

https://ocw.mit.edu/courses/18-06-linear-algebra-spring-2010/