Help With 5 Axis Toolpath Recommendations

[McLaren]

I was wondering how you would come at machining the inside of this part. The floor radii are .125" and the pocket is almost 3" deep on the left side, and just over 2" deep on the right side. Last time I did a part similar to this after roughing I did a ton of Flow 5 Axis toolpaths using Tool axis control - From point, and just guesstimating where a good 'from point' would be. I am hoping someone else has a better solution. Thanks for looking!

[Guest]

Can't query the geometry as just a pic but looking at it...I'd say you have a mostly 3+2 part there

 

[McLaren]

 File attached if you want to take a look. The 'OP3 5 AXIS' group is my old one that I want to improve on. For sure I will use OptiRough this time. My main concern however is a 1/4" ball endmill hanging out over 3".

0002021 0002037.ZIP

[Guest]

3 minutes ago, McLaren said:

My main concern however is a 1/4" ball endmill hanging out over 3".

Why not a bull nose with .125Rad

[McLaren]

Far left and right sides are .125" corner and floor radii.

[Guest]

4 minutes ago, McLaren said:

Far left and right sides are .125" corner and floor radii.

That's fine, myself, I would use a lager tool where ever possible and only blend those areas I needed.....

One 5 axis, you would certainly tilt and make the reach a little easier

Come into the corners like this instead.....allows you a larger tool and provides easier access with what should be a bit of a shorter tool length

[Aaron Eberhard]

Normal disclaimer in effect:  This method is the "best/fastest/safest" method I've found, but it's not the most efficient from a raw machine cycle time.  If you're cranking out a bajillion of these things, it's probably worth the time to optimize to individual features (handle this wall all in one go, then switch to the other, etc). 

How I like to try attacking features like this is to try to use a "fixed angle to axis" tool axis control with collision control set to "tilt away to avoid gouge > Automatic."  That will give me a "3 axis" toolpath that will tilt away to avoid hitting when necessary. 

I started with a Parallel set to  "Parallel to:  Constant Z."  That will give you a Waterline-like toolpath, tune your tolerance and step down to your liking.  I'm cutting the entire inside (painted green here):

Next, on the tool axis control, I set it to Fixed Angle to Axis : Z (this is the OP3 B0C0 WCS, so I want the tool to align to this WCSs' Z axis).

That was followed by a stop on the Collision Control Page to ensure that everything was gouge checked, and it was set to tilt away.   Note:  You'll almost always want to visit the Tool Clearance page to ensure that it's not over-tilting due to the clearance distances being too big.  2018 makes this easier:

Finally, it's time to clean up the linking.  I set this to blend a "small" gap.  For my purposes, I wanted it to keep down when traversing the circles cut into the part, but feel free to retract up a bit when it comes to the long gap in the pocket.  When it's coming to a big gap, I turned on lead in/out, so it arcs away nicely.  This is covered by the blending motion on the small gaps, so it's not really necessary there:

 

That gives me this:

 

Now, to be fair, I spent about three times longer writing up the walk-through than actually programming the part, so there's lots of room to tweak it to what you need, but it should get you down the right path.

Oh, and one other note:  I've found that when I'm trying to get smooth motion around a fillet, especially one in multiaxis, it helps to give it the real tool diameter (probably .2496 or 97) instead of .25, since now there's no room for the toolpath to adjust tilt mid-corner as it's in a perfect fit situation.  If you give it a little bit to play with (that exists in the real world anyway), it'll help "smooth" out the corners a touch.

 

Hope this helps.

Automatic tilt Away - 0002021 0002037.zip

[McLaren]

 That's fantastic, thanks a ton! Definitely gives me something to play with, and solves the issues I didn't like about my original process.

[McLaren]

 Aaron, any thoughts on why I can't prevent the tool holder from colliding? If you look at the files toolpath ID 283 is what I thought should work, 282 is messing with numbers to see how they affect the backplot. I have collision control and tool clearances set up, as well as check surfaces, but it seems to ignore the end of the holder.

0002021 0002037 COLLISION.ZIP

[McLaren]

 Problem solved. I created a new surface offset from existing solid and am using that as my check. Still curious why the old surfaces weren't being honored though.

[Aaron Eberhard]

I think that was a defect discovered early during beta of 2018, if I recall correctly.  The issue was that it ignoring the tool projection and going off of the whole length of the tool.  I just opened the file and regenerated op #282 and it is no longer in collision.