Finishing sphere, on a 5-axis

[Grimes]

Well, got a new job on an okuma 5-axis mill this week. I know jack about the machine, but they are willing to train.

Today we were trying to get a smooth finish on a part with a ball on one end, first trying to use a dove-tail cutter but nothing was working right. A few people were scratching their heads on it. We were trying waterline, and raster. They both wouldnt do the undercut. In the end it was done using a ball endmill using raster but only one half at a time. It left a small step where the two halfs met. Just curious what tool should have been used and which toolpath, as i know nothing, this is just to show the guy training me how we should have done it, if another similar part comes up. Thanks

 

Bit more info ball, was .250 +.002

 

Also, there will be more questions as i get more comfortable on the machine lol.

[Greg Williams]

maybe easier with a mastrecam file

[Jespertech]

This is a part that I cherry picked from another topic on this forum last week. I  just completed my multi-Axis class at MacDac (my local reseller) and have been trying to get as much  experience as possible with different parts and toolpaths. You have to remember that there are "99 ways to skin a cat" and this is just one possible approach. Different toolpaths will produce varying results depending on the machine and setup. But I'd recommend digging deep through Emastercam and reading all of the posts that relate to multi axis finishing etc. It has been by far the most helpful resource in my programming apprenticeship. 

BALL TP.ZIP

[Grimes]

Just wondering on the legal side of things, one prototype, and they wouldnt allow you to have your phones around it in case you took a picture.

[Jespertech]

2 minutes ago, Grimes said:

Just wondering on the legal side of things, one prototype, and they wouldnt allow you to have your phones around it in case you took a picture.

yea, that can be tricky. You can try  to recreate just the feature in question and post that. 

[crazy^millman]

Dovetail cutter trying to cut the part yes not my first or even tenth choice for trying to cut a sphere.

Ball endmill yes, but I would have used a 5 Axis toolpath and not a 3 Axis toolpath. Sight unseen hard to point you in the right direction. Get some training from your reseller or one of the Online companies offering it. This site offers training, CAMInstructor, Streaming Teacher and Mastercam U are some I recommend for different things.

One way to Machine the Sphere

Jespertech Here is your file with a little different spin put on it. I used Unified to cut the part and then I added a 1/2 ball endmill to go back and chase the 1/4 radius at the transition. Hopefully it give you something more to use in your learning.

[Colin Gilchrist]

Are you looking for something like this?

Driving a spherical surface, using a 5-Axis Toolpath?

Mastercam has a very sweet new 5-Axis Path called "unified". I used the Automatic Cut Pattern method, Style > Center - Morph. I selected the spherical face as my machining geometry.

Cutting Method > Spiral

Under the "Guide Curve - Advanced Parameters" Page > Projection Direction = Surface Normal (This is what points the "cut pattern towards the sphere").

The Tool Axis Control [TAC] = Surface with Tilt (this is a "surface normal" stragety.

> Under Advanced Options (TAC) > Gradual Side tilt angle change = -6 (This is really helpful, as the tool starts "normal" towards the tool axis control surfaces. As the tool "spirals" from the surface edge, towards the "top tip", we start to reach the "singularity" on a 5-Axis machines. (This is not where gravity becomes so strong that it pulls in all light except for what is excreted 

Sphere-5-Axis-example.mcam

[Colin Gilchrist]

I had typed out just a little more to this initial reply, but I think my window got closed, and I lost some of the text.

A "singularity" is a situation where the Rotary Platter on a Trunnion Machine (C-Axis Table, is typical here), is sitting "flat to the spindle face". (Tilt Axis is "at Zero".) When that occurs, some interesting problems can arise "mathematically", so it is best to avoid these situations completely.

In Layman's Terms: When programming a 5-Axis "Vector-Based" Toolpath, avoid "vertical vectors" (0, 0, 1), in the middle of the toolpath. Having one at the start, or end, can be "ok", depending on "how the rotary was positioned prior to the current toolpath being executed on the machine, and the interaction of about 200+ Parameter Values, depending on your Control Type.

With all 5-Axis paths, you really need to look at the output of the code, for each path being Posted, if you aren't using Verification Software. Even if you are using VERICUT, NCSIMUL, or another Simulation Solution, the "NC Code output" in Mastercam is designed to be controlled by the Programmer, by using the Miscellaneous Integers and Decimal Numbers (Real Numbers), at the Operation Level. This means you can "tweak the MI/MR values", and "force a Regeneration of the Path", and you will get different NC Code Output, based on the MI/MR Values: "Passing Data to the Post".

By using the "Positive or Negative gradual Side Tilt" option, we can "start normal", but then progressively add a little tilt to the tool, to expressly avoid that Singularity Situation (AKA: The black-hole of 5-Axis Programming! Lol)

[So not a Guru]

22 hours ago, Jespertech said:

This is a part that I cherry picked from another topic on this forum last week. I  just completed my multi-Axis class at MacDac (my local reseller) and have been trying to get as much  experience as possible with different parts and toolpaths. You have to remember that there are "99 ways to skin a cat" and this is just one possible approach. Different toolpaths will produce varying results depending on the machine and setup. But I'd recommend digging deep through Emastercam and reading all of the posts that relate to multi axis finishing etc. It has been by far the most helpful resource in my programming apprenticeship. 

BALL TP.ZIP

For the axis control on this "To point" is selected. Where is the point and how is it selected?

[Jespertech]

2 hours ago, So not a Guru said:

For the axis control on this "To point" is selected. Where is the point and how is it selected?

I believe I just selected the center point of my rotary. I should have made a separate level with an actual created pt for reference though. I can see how not having that information isn't very helpful... I also deleted pretty much everything (levels , fixtures etc) out of the file in hopes to be able to post it, but I had to create a zip file anyways because it was still too large. So that too is why the point is nowhere to be found.

[Grimes]

Gonna upload the modded file tonight.

[Colin Gilchrist]

On 1/6/2022 at 8:47 PM, Grimes said:

Well, got a new job on an okuma 5-axis mill this week. I know jack about the machine, but they are willing to train.

Today we were trying to get a smooth finish on a part with a ball on one end, first trying to use a dove-tail cutter but nothing was working right. A few people were scratching their heads on it. We were trying waterline, and raster. They both wouldnt do the undercut. In the end it was done using a ball endmill using raster but only one half at a time. It left a small step where the two halfs met. Just curious what tool should have been used and which toolpath, as i know nothing, this is just to show the guy training me how we should have done it, if another similar part comes up. Thanks

 

Bit more info ball, was .250 +.002

 

Also, there will be more questions as i get more comfortable on the machine lol.

Something to note:

If you're programming a machine without advanced 5-Axis Cutter Compensation available, you will need to edit your Tool Definition to 0.252, and not just the "0.250" nominal size. This is due to how the compensation works. On a sphere, you can probably get away with just adjusting the Tool Length Offset value, to compensate for the size of the sphere. But if you had a complex set of free-form surfaces, and you were 5-Axis machining, you'd want to have your Tool Definition in Mastercam be as close as possible to the actual dimension of the tool "in the real world".