Ball Mill Advice

[electrosteam]

I am 3D Profiling tapered oval spokes in Cast Iron wheels for a 5 inch gauge locomotive.

5 mm end mill, 0.5 mm clearance, followed by 5 mm ball mill, 0 mm clearance.

The spoke oval profile produced is wrong, correct overall size but the side curvature is too sharp.

A 5 mm end mill, 0 mm clearance, is the correct size and profile, but shows the depth steps.

Just looking for advice and suggestions on where to look for hints on how to mix and match end mills and ball mills.

John.

[lloydsp]

You almost caught me by surprise.  I 'wrote the book' (actually and 'literally') on ball milling in amateur pyrotechnics.  When you wrote 'ball mill advice', the old stuff rushed back, until I realized you meant 'ball-end mill'.  (In that parlance, a 'Ball Mill' is a device for finely grinding chemicals, using a rotating drum full of hard grinding balls with the chemical among them. <grin>)

We can't help much without seeing some images of the cuts -- how they should be, how they turn out wrong, and copies of the geometries and MOps creating them.

I've never had difficulties getting a ball-end mill to conform to a 3D surface, so I can't picture what your problem is.

Lloyd

[dh42]

Hello

as said Lloyd, we needs more infos ... the better is to share your file so we can experiment and simulate ... 

++
David

[electrosteam]

I previously posted an image of the wheel model on 03Jul25.

Attached is an image providing a rough idea of my observation.
I think my problem is incorrect set-up of CamBam and/or milling machine.
I have started reading the French Documentation, hoping to get some guidance.

I have mounted a test-piece on the machine and trialling cuts on a single spoke.
Most of the two adjacent pockets is present so the tool engages the spoke correctly.
Keeps development and job times bearable.

(A) Waterline Roughing cut was made with 6 mm end mill with 0.5 depth of cut.

(B) Waterline Finish with 5 mm ball-end mill.
I selected "Ball Nose" for the tool and 4 flutes, but left all other tool entries at 0.
Nominated:
 - Depth Increment 0.2,
 - Max Crossover Distance 0.2,
 - Resolution 0.2,
 - Roughing clearance 0.1,
 - Stepover 0.2.

Results in the bulge depicted in the image.

(C) Waterline Finish with 5 mm square end mill.
Nominated:
 - Depth Increment 0.2,
 - Max Crossover Distance 0.2,
 - Resolution 0.2,
 - Roughing clearance 0.1,
 - Stepover 0.2.
 
 Result after (C) is a good representation of the tapered oval shape.
 The end mill cleaned out the bulge left by (B).

Are my CB selections in (B) reasonable ?

John.

[dh42]

Not sure to really understand, but I see at least on thing wrong, roughing clearance must bee = 0 for finishing.

Also you can try a resolution of 0.1 for the ball nose to get a better approximation of the tool profile.

Be sure you select "Ball nose" and not "Bull nose" for the tool profile of the hemispherical mill. ("Bull nose" is not yet supported and give the same result than "End mill")

for summarize to be sure I understand

The profile that you want is the one in green and you get the one in withe ?

You get the right profile when using a (square) endmill ?

It would be great if you can share the .cb file itself ..  it is more easy to find the Gremlins !!

++
David

[electrosteam]

Thanks for the comments.

The Roughing Clearance could be the problem.

Desired: White,
Actual cut: Green.

Definitely " Ball Nose".

The square end mill gives the correct profile.

Just setting up to redo the 5 Ball Nose, with Roughing Clearance 0.
I will leave Resolution at 0.2 so that only one thing is changed.

John

[electrosteam]

Two tests:

1. Existing Spoke:
Spoke previously cut with 5 mm end mill Waterline Finish and Roughing Clearance 0.1 mm that gave a good profile.

Run with 5 mm Ball-end mill with Roughing Clearance = 0 mm.
The Ball-end mill barely touched the surface.
So, possibility is that the previous incorrect Roughing Clearance caused some errors.

2. New Spoke:
New stock with 6 mm end mill Waterline Rough, then 5 mm Ball-end mill Waterline Finish.
Roughing Clearance = 0.5 mm for WR and 0 mm for WF.

Same result, spoke comes out with the previously reported "bulge".

My set-ups are repeatable, just wrong.

I have a friend who is an experienced CNC operator visiting in a couple of days.
We will review everything then.

At the moment, the best result is with a square end mill.

John.

[Tool-n-Around]

For comparison, have you tried horizontal and/or vertical scanline 3D MOPs with the ball end mill? At minimum the tool paths will generate in a small fraction of the time compared to waterline, and if you can increase the resolution and reduce the step over to say .1 for each, to produce the finish to suit, but if you simulate doing so, you can at least see if the shape error is limited to waterline MOP.

I gave up on the WL MOP in CamBam except for roughing with square end mills. Instead I use horizontal or vertical (sometimes both) in selectively bound areas. -Very fast to simulate and prove program, and just works every time.

Best,
Kelly

[dave benson]

John
I made a spoke stand in model in Freecad, its a nice low res file that will take a couple of seconds to generate tool paths for.
Before I exported the file I checked it with the analyzer in the mesh workbench.

I then imported it into CB and applied a 3D mop to the model.

I did as little as possible to modify the mop just target depth and tool and I also set the stepover so it shows in the simulator.

With the model I used the selected boundary shapes method and added the polyline as a boundary shape.
This stops the tool diving down at the end of the shape in the sim.

In the first pic 'spoke stand in' the toolpaths have been generated, they are the blue lines, they represent the center line of the
tool not the cut surface, in this example they are ok.
In the second pic 'spoke stand in ok' is a representation of the surface after machining.

Like all trouble shooting, start at the beginning the model must the watertight.

In Freecad you must check where the spoke shape joins the hub as the filleting fails sometimes.
What this causes is a file that takes a long time to export a long time to import and forever to generate the tool paths for.

I did a sanity check and exported the cut surface from camotics to CB and superimposed the two surfaces to get a visual comparison and it looks ok.
Dimension wise.

Sometimes you get problems if you have set the boundary objects to close to the model and there is not enough room for tool clearance.

If you generate your code and the tool dives down to the target depth at the end or start of the model
it will be caused by the model being rotated off axis by any amount, the model in my file that works well, if I rotate it even less than a degree in Y it will exhibit
the steep dives into the work piece which will break the tool.

Dave

[electrosteam]

Kelly, thanks for the comments.
I had seen some of your contributions and I was considering the possible use of Scanlines.
 
I am spending time reading documentation and searching old threads.

The problem undoubtedly is one of misapplication, so I am sure it will be solved.
There are so many variables and ways of approaching the problem, I just need to learn more.

Dave, thank you for the work you have done, it is a great example.

But, there is a fundamental difference to my job, the wheel spokes are tapered for both width and height.
I will duplicate your example with one tapered spoke as a test.

Don't worry, FreecAd and I are old friends (protagonists?) dealing with fillets.
And MeshLab and I are starting a great relationship, with Blender commenting from the side.

Thanks for showing the Camotics simulation with a ball-end cutter.
It prompted me to review the tool table in Camotics so that my future simulations will show the correct tip.

John.

[electrosteam]

I duplicated Dave's example, but with my tapered oval spoke, and a 5 mm ball-end tool.
Result was the excess "hip" in the machined curves,

Re-did with a 4 mm square end-mill, 0.1 depth step, and got a good approximation to the desired surface.
I think filing/emery paper will provide the correct shape.

Unfortunately, I have come to the same conclusion as Kelly, the Waterline Finish MOP with a ball-end mill has issues.
The Forum history has numerous discussions on problems with ball-end and Waterline Finish.

My understanding of the Documentation description of the ball-end algorithm almost guarantees incorrect machined surface for tapers like mine.

But, there is always another way !
I am exploring a mix of MOPs as suggested.
Drilling for chip evacuation, pocketing to get close, ball-end WLFinish to get all the fillets, and a final square end mill on just the linear part of the spokes.
The fillets only have to "look" nice,

I use LinuxCNC for the machining, and I have tested its co-ordinate rotation responses to be comfortable with its operation.
So that is simply a MOP subroutine called 8 times, the number of spokes, at 45 degree increments.

As a side note, if you search for a more general discussion of ball-end algorithms, you discover wide-ranging discussion for all the major machine and cam products.
CamBam is normal for the problem.

 John.

[dave benson]

John

As a side note, if you search for a more general discussion of ball-end algorithms, you discover wide-ranging discussion for all the major machine and cam products.
CamBam is normal for the problem.

Yes there are common issues across all cam and cad programs, for example the malformed radii
where they are too close has been spoken about in the fusion forums.

In pic one is a model, Its a low res one that shows one of the problems that you can have using a waterline mop to duplicate a surface faithfully.

The first pic is of geometry from a game (an island and beach)
The problem is that the beach area which has a  largely flat shallow angle so the spacing between tool paths is too sparse which
will leave uncut areas, intuitively you might decrease the depth increment this works but increases the cutting time massively.

This is a problem with the waterline method and also applies to 3D printers where they have solved the problem by making paint
on tool paths (layer height) which can be varied in just the areas needed. I have used that technique to achieve good results while making spheres.

In the other pic is a shot of a pocket followed by a 3D mop (waterline finish).
The wheel is 96 mm dia and the tool diameter is 3mm, it takes 2 hours for 3D mop. I've used the values I would use to cut mild steel.
About 3 hrs for each wheel.
The Hornby wheel has a flat back side so you would have to turn over the model so would need some form of indexing.

I use Mach3 so tool changes are a breeze to do, the 3mm tool that I used in the pocket mop
I would swap out for a larger dia flat bottomed end mill which would remove the bulk material
much faster.

I think you said earlier that the wheel was 5 inch in dia, so about 130 mm.
This would lend itself to a combination of 2.5 and 3D mops.

With the Hornby wheels, they are all ok regarding the radii problem and are drawn in freecad
at the correct co-ordinates and importantly are attached to a plane face, flat with no angular deviation, as this will cause problems in cb.

I will post the file so that you can have a look.
I did do another scratch file at the time using the spoke stand in and put a taper on it, it was ok too.

At this point its hard to tell if your model is the problem or a simple mop setting.
If the model is proprietary whip a stunt double (changing the dimensions and spoke geometry) just so that it is similar, this way we can
check if the model you have drawn in freecad (the stl) is ok for CB.


Dave

[dave benson]

couldn't fit all the pics and the CB file.

[electrosteam]

Thanks Dave for those images and the CB file.

The way you added multiple polylines to guide multiple MOPs is just what I was heading towards.
Your example shows that this approach will work.

I am intrigued with the polylines following contour paths.
A ball-end mill following these polylines may give a perfectly acceptable result.
I will get some time soon to try some MOPs on cast iron test pieces.

How did you produce these contour polylines ?

John.

[dave benson]

Here you go.