CAM generation for 2D Adaptive Clearing taking hours with fairly simple geometry

[Anonymous]

Hoping someone can help me with the issue of 2D Adaptive Clearing taking a very long time to generate toolpaths. I have uploaded an example file which is one of the more extensive toolpaths.

I expect it to take long, but it is currently not uncommon for toolpath generation to take longer than than the machine takes to cut it; in a machine that is not HSM capable, mind you.

I uploaded screenshots showing the selected geometry and pass parameters as well as the generation progress so far.



Specs:

2.0.10564
Active Plan: Fusion 360, Student
Windows 10 (19042)

[seth.madore]

Could you share your file please?
File > Export > Save to local folder, return to thread and attach the .f3d file in your reply

[Anonymous]

I'm not sure why but I am not finding a way to attach the file. I only see options for me to attach a picture or video.

[seth.madore]

 

[Anonymous]

I don't have a box to drag and drop to other than the dialogue box and it shows this message:

[seth.madore]

Go back to the forum thread. At the very bottom is this chat box:

 

Click on it and it will expand into something you can type and upload stuff

[Anonymous]

Ah I see. For whatever reason, that option isn't available when you click reply. Thank you again.

[seth.madore · Accepted solution]

Umm....

It's your Optimal Load. Are you machining/grinding ceramic or some other super brittle material? .0008" load is not very good for tools, especially since it's doing a roughing toolpath. In a commercial VMC, I'd expect to run in the .02" range, depending on material (sometimes more, for soft stuff)

[Anonymous]

It's a 0.1406" AlTiN coated carbide cutter cutting into 52-100. I've been taught to keep the engagement low and feed rate high to maximize tool life and utilization. When we were doing engagements around 0.01" with a 0.5" coated carbide endmill, it sounded extremely rough and we were running through endmills like nobody's business

If I have my engagement at 0.02" but my feed per tooth is set at .002", will it maintain that chip load per tooth at that engagement? I suppose this is where I am mainly confused. Apologies if this is a super simple question but again I am newly learning this.

I should also add the machine we are using is a Trak 2OP

[seth.madore]

Is this heat treated 52100 steel? I've never personally cut it (aside from milling some flats on a shaft a long time ago)

It's looking to be about a 40% machinability rating in the soft state. Do you have recommended speeds and feeds?

At any rate, .0008 is way too light of a chip load. I certainly wouldn't go to my suggestion of .02", but perhaps in the 5-6% range

[Anonymous]

It has not been heat-treated or hardened. In it's current state I am told it runs about 38 Rockwell. Thank you very much for the info, I will be meeting with my team about the chip load being too minimal.

As for speeds and feeds I typically use the FSWizard app and adjust from there based on the sound. 

Example: a 1/2" AiTin coated carbide endmill with a corner radius of .02" will commonly run with a spindle speed of 2889 and a feed rate of 40-50 in/min for an FZ of .0035-.0045

Did quite a bit of research on the subject and read a lot of accounts of people milling in the same material who have the same recommendation as yourself. I will post an update once we have dialed in the new parameters and gotten our feed rate optimal.

Thanks again!

[seth.madore]

You say it's 60-65 RC? Holy smokes my man, that IS heat treated

[Anonymous]

SORRY! I had to edit. I was basing it off of Google which doesn't show the untreated hardness no matter how I word my search. My superior came in and expressed that they usually test at 38 Rockwell C. My mistake.

[seth.madore]

Okay, that makes more sense now. What is the machine you are using, and do you have coolant?

[Anonymous]

It is a Trak 2op 3-axis VMC made by Southwestern Industries. Not HSM capable with a max spindle of 10,000rpm and max cutting feed rate of 99in/min. We have 3 coolant nozzles flooding coolant anytime we cut.

[seth.madore · Accepted solution]

Right, you mentioned that above, sorry about that...

Do you feel that the machine is durable enough to be doing this machining? How does it sound, is it squealing or making a smooth cutting noise? What color are the chips, and what does the surface finish look like?

Changing the Optimal Load to .005", generation took 189 seconds. Now, that's not a crazy low number, but given the cutting parameters, it's something I'd say is to be expected. The other option that's on the table would be to use 2D Pocket with small(ish) stepovers. YMMV though..

[Anonymous]

I think a big mistake on my end was trying to match the sounds of the much more rigid and fully HSM capable Robo-Drills and Kiwa machines on the Manufacturing side (I am in the smaller customs and prototyping shop for our company.)

It sounds good and is making a consistent cut. I've attached photos to show chips and surface finish. Going to tweak my lead-out a bit but otherwise this has been quite the game changer of a lesson for me.

My once 18 minute op is now 1.5 minutes. My chips are chips and not simply dust.

Look at me, Ma I'm machining 😄

[seth.madore]

That's awesome! What did you settle on, or are you still proving out the recipe?

[Anonymous]

Still fine-tuning it but right now, since we have endmills with a LOC that is far too long, we still have a bit more deflection and harmonics than we should. This is something I have addressed and we will be changing to further help with optimization for our particular needs. Generation time problems appear to be in the rear-view at this point. Very happy with the result so far.

Currently running 0.5" AiTin coated bullnose endmill with a big .09" radius on the edge. Running at 2889rpm and 50in/min max cutting feed rate ending up at a FPT of about .004"

DOC: .06" & .150"
Optimal Load: .02

Tolerance: .004

Smoothing Tolerance: .002"
Radial stock to Leave: .01"