Issues Machining Small Parts (Smaller than 5 mm)

[BH-LLC_Jay.Russell]

I'm machining small, acrylic, intraocular implants for work and am having issues with the paths that the CNC Mill is following. The mill is a MicroMill DSLS 3000, and I'm controlling it using Mach 3 on a 64-Bit, Windows 10 laptop.

I'm able to use the 3D operations to machine all of the contours just fine - and I'm quite impressed with how well they guide the 1/64" ball mill I'm using. I've been able to push it to a feed rate of 40 IPM! It's the 2D operations, however, that give me the issues.

Because of our patent situation, I can't go into a ton of detail about what the design looks like. But, the basic profile that I need to cut out using the 2D operations looks like a kidney bean. The implant, and, therefore, the profile, is symmetric and the toolpaths that Fusion generates reflect that. The issue I'm having is that the profile cut by the machine is lopsided, i.e., one side of the kidney bean is larger than the other. The width of the profile is 1.55 mm in Fusion, but, the profile cut by the machine goes from 1.45 mm to 1.65 mm. I did a brute-force fix of this by cutting out the center arcs, offsetting each end by the corresponding error, and then re-joining them with tangent arcs (see attached screenshot). This got the sizing consistent, but there are still numerous other issues with the shape of the profile, e.g., non-tangent edges at either end of the profile, and other jagged changes in direction.

Has anyone seen anything like this before?

Thank you!

Jay

[Marco.Takx]

Hi @BH-LLC_Jay.Russell,

To help you the best you can do is to share your model so we can take a look at it?

note us witch operations have issues so we can analyse it. 

[LibertyMachine]

@Marco.Takx he expressly stated that he can't share the design 😉

@BH-LLC_Jay.Russell would it be possible to do the following:

Perform a "Save As"

De-Feature the part. Go through and delete a whole bunch of stuff that still leaves the perimeter intact.

Share that file with us? (File > Export > Save to local folder. Return to thread and attach the .f3d file in your reply)

Is Smoothing turned on? How is the chain selected, by sketch or solid model profile?

Lastly, I'm more than willing to sign an NDA and have you invite me to the project. It's something I've done countless times for other community members.

[Marco.Takx]

Hi @LibertyMachine,

I know but with only a screenshot without any more detail it’s hard to help. 

@BH-LLC_Jay.Russell If you can’t share your model maybe it’s a solution to contact your local reseller. They can maybe help you remote solving the problem. 

[daniel_lyall]

That is a strange problem I have never seen a 2D cut in Mach3 do that, 2.5D or 3D it can happen when you are going to fast for all 3 axes to keep up.

One thing you can try clean and lube the machine and double check it is squire if it is sticking or out of squire it can move one end more than the other. 

other than that what Seth suggests is a good option just posting the profile a second set of eyes can help most times.

One more thing you can try just sketch the shape in a new file and see if the machine does it when all there is just the single sketch, a traces or profile will work just make sure you set a depth for it an mm or 2 would be enough. 

[BH-LLC_Jay.Russell]

@LibertyMachine, @Marco.Takx, @daniel_lyall:  Thank you all for your willingness to help! I've attached a defeatured model, containing the toolpaths in question, for you all and the rest of the community to take a look at.

I think, by simply creating this defeatured model, I've figured out the issue. Though I initially created the geometry by only using arcs and straight lines, the contoured nature of the implant (which I removed in the defeaturing) causes the profile to be partially generated with control point splines. You'll notice that the large, rounded faces have splines interrupting them instead of them being one, continuous arc. I'm going to rebuild the profiles using only arcs and lines and see if that changes anything. I'll post an update once I have the results!

@LibertyMachine:  To answer your questions in detail:  Smoothing is turned on, but it really doesn't change that much. I have to make the smoothing tolerance much higher than the base tolerance for it to recognize any arcs in the profile. By then, it's too far gone from the original to be of any benefit.

I've selected the profile by directly selecting it off of the model, as well as selecting a sketch. The sketch was generated by projecting the geometry, though, so it contains many of the splines that the direct, model profile has.

@daniel_lyall:  I, too, thought speed may be the issue, since I'm pushing these small tools to 40 IPM. I tried cutting the profile at 40 IPM and at 10 IPM, and the machine produced identical contours. I've squared the machine as well.

[BH-LLC_Jay.Russell]

After my testing with the new contour, it seems like I may be having issues with backlash. This isn't my machine, and I have no idea of the maintenance history on it. So, I'm going to measure the backlash and enable the Backlash Compensation feature in Mach 3.

Have any of you all used this feature before? If so, any experiences you can share with me will be much appreciated! I'm mostly just a YouTube scholar when it comes to this stuff, so I'm open to any suggestions.

[daniel_lyall]

I know of a few people that have tried to get backlash working in Mach3 they all gave up and fixed it on the machine.

[BH-LLC_Jay.Russell · Accepted solution]

Well, now you know another person who did the same thing! =P

I measured over 5 thousandths of backlash in the Y-Axis of my machine. So, with the help of a coworker, I took it apart, adjusted the lead nut for the Y-Axis, gave it a thorough cleaning (which it needed badly), and put it back together. I've made some test cuts with it today, and that seems to be the issue! The backlash is still around 1 thou on both the X and Y axes, but that doesn't seem to cause any issues.

Thank you all for your help!