5TH AXIS POSITIONING

[dan73]

Hello

I have a large piece on a HMC boring mill w/5th axis ©. The part is too big to mill without over traveling. I need to mill a section then rotate my C-axis 120 degrees and repeat, something which I have done before but long ago. I think I tried every combination in the transform/rotate tool paths. I tried to set the machine limits, but that had no impact in the NC file. Is there something simple I am missing? Is there something wrong with my post? It is a custom 5 axis HMC post from my reseller,But want to make sure I am not missing something before I contact them( I need help ASAP). It doesn't seem like it should be this hard! I figured out a hundred different ways to "cheat" it, but want to know the right way.I am using X5.

Any help would be appreciated.

[gcode]

did you try rotating your toolplanes about Z 120°

[dan73]

Yes. That was the first thing I tried. Made no difference.

[K2csq7]

Dan, you said it's a custom post...

In your misc integers, do you have "initial primary"?

 

using G's rotating t/c planes in conjunction with putting in the same rotation for the initial primary gave me what I think you need.

[dan73]

I don't see "intial primary" in the integers, but i do have "intial rotary axis position" in the misc. reals. I tried to change it to 120.0 but had no effect. I will try changing that and rotating my T/C planes.

 

If I rotate both C and B axis in the tool plane everything works great(as to drill in the side of the part). I tried other posts/ machines and none would give me the desired results.

[Chris McIntosh]

I'm assuming this is a 5-axis toolpath that you are trying to rotate. Did you try transforming by coordinate instead of toolplane?

 

Hard to say what the issue is without seeing the part.

[dan73]

No they are simple 2d contours and then some drilling. I just need to make the parts in section, because we took on a part much larger than our capability (sound familiar everyone?) The post actually came from you guys up there. I cannot get the post to rotate 120 degrees about the z axis to repostion the part. I must be missing something simple.

[Chris McIntosh]

I'm a little confused as to exactly what you are trying to do....whether you want the post to automatically rotate the part in the middle of a 3-axis operation or whether you've split the operation up into multiple operations.

 

The position of the rotary axis is controlled by the toolplane for these positional toolpaths. If you are expecting the toolpath to rotate the part in the middle of an operation, that's not going to happen on a 3-axis toolpath.

 

If you are repeating the same cut at the initial position, then repeating it 120 degrees away, you should just use a transform rotate toolpath (make sure you select toolplane rotation).

 

Otherwise just define a new toolplane that is a 120 degree rotation about Z of your original toolplane and program the next cut.

[K2csq7]

Here is a file with stock MD, CD, & post.

 

I drew a circle at the bottom of my screen (y negative) toolpathed it, then created a new view (new view 8) by rotating plane (180about z), switched the planes in the op to the newly created one, then on the misc values page I put in the 180 (I know u said 120 but I don't think there will be a difference). posted and I get "C180" and the contouring is happining in the Y positive direction (180 degrees from where I drew it).

 

Is this what your trying to do, or did I miss the boat?

[dan73]

"If you are repeating the same cut at the initial position, then repeating it 120 degrees away, you should just use a transform rotate toolpath (make sure you select toolplane rotation)."

 

"Otherwise just define a new toolplane that is a 120 degree rotation about Z of your original toolplane and program the next cut."

-This is exactly what I am trying to do.

I have tried both of these ways many,many times.

 

When TRANSFORM Rotate everything looks good in the graphics window, but I need the rotary table to physically turn 120 degrees or else i will run out travel on the Y axis.

 

When I create a new toolplane rotating about Z, there is absolutely no change in my post. It will cut the same contour, in the same place without rotating the part. I am using a horizontal miller,with a rotary rotating about z axis, and my planes are set to WCS=top

Tool=front, Comp/const=front.

 

When I create my new rotated plane, I change my Tool and Comp plane to "new view"

I believe I am doing everything correct.I work with 4th and 5th axis all day long, but never had this situation before.

[Chris McIntosh]

Can you send me the file with your post and I will look at the programming/post to see what is going on?

[dan73]

Yes. How and where should I send it?

[Chris McIntosh]

just sent you a PM with my email addy

[dan73]

Kieth-thanks, but I could not open your file for some reason. It sounds like what I am trying to do and everything I did. It just will not post out the C moves.

[Chris McIntosh]

Just saw what Dan was programming. The issue is that he was machining in the same axis as he was trying to rotate about so the post had no way of knowing a rotation was necessary. I enabled the twisting option in his post with a few modifications and now he should be getting the right output. Just a solution update!

[dan73]

Thanks Again for everyone's help! Really appreciate it! Problem solved, Thanks Chris.

[K2csq7]

I tried a couple more things with the file I had up there. (Sorry you couldn't open it Dan????)

My method worked fine for 180 degrees, but when I tried 120, it would still rotate to 180. It still gave me usable rotations & the correct X, Y locations, but I could not get it to start at anything but 0 or 180.

 

I enabled the twisting option in his post with a few modifications

Care to share Chris? Sounds like something I could use... I do a lot of drilling keeping the spindle at X0, Y(negative whatever) and just rotating with the C axis. My 5ax post wont do this for me so I need to keep an entire separate post, MD, & CD.

[Chris McIntosh]

Our post uses the tool plane to calculate the c-axis rotation when your tool is parallel to the machines axis of rotation. So if you have a C-axis (rotation about Z) and your tool is vertical (along the Z-axis), any C-axis value is technically achievable. So we built in a function to allow the user to control the C-axis rotation based on the rotation of the plane. If you take the top plane and rotate it 90 degrees, the post will identify this and rotate the C-axis 90 degrees. In our post this is enabled through a switch called "use_twist".

[Jeremy Herron@DBS Solutions™]

I also have an inhouse post and use_twist output correctly, but lets say I needed to chamfer a 35" o.d. and because machine limits I needed to start at what would c225 or c315 and cut with c all the way around like a c-axis face contour on a lathe? Is that possible? I know how to do it with a 5-axis toolpath, but it would be nice to be able to use 2d chamfer.

[K2csq7]

I don't know about this "use_twist" thing, but I use a 4 ax post for stuff like this.... axis sub rotate about z.

Maybe the Axis sub will give you what you need.

[Jeremy Herron@DBS Solutions™]

I tried Keith, but no go. I did not really figure it would from Chris's explanation of use_twist earlier, but it was worth a shot. I can do it with a 5-axis toolpath by kicking my tool axis off just a little, or go to a-90 and be normal to the o.d.. I was just trying to keep from drawing all the extra stuff for it.

[K2csq7]

Could prolly get it with a curve toolpath locked to 4 axis & use axis limits.

edit: nope

 

Wish the 5 ax posts had an option to "pretend this is only a 4 axis machine"

[Jeremy Herron@DBS Solutions™]

That would be AWESOME! but there is plenty of other stuff I need fixed before that, but this not the forum for that.