Adaptive clearing feedrate enhancement

[avantmfg]

Hello,

Well I am not currently an Autodesk user but am looking to make the switch to programming with HSMworks. I have some ideas for features which if incorporated into the software would make it that much more enticing for me to switch sooner rather than later.

My first idea has to do with roughing. In a constant engagement angle style roughing toolpath with both step-downs and step-ups, the load and material removal rate while cutting decreases with each successive step up. An opportunity lies in increasing feed with each step up. For example, if I want to cut 1.0" deep axially with each step down, then step up every .050", there are 20 cuts of various axial cut depths but each successive cut is .050" less than the preceding. If I had set the feedrate to 400ipm, which made for acceptable tool load and material removal rate on the 1.0" deep cut, by the time I have reached a cut depth of say .200" a faster feedrate would be preferable.

In my mind, this is a very simple feature to implement without over-complicating either the work on the developer's end nor the usability for the machine programmer operating the software.

A field for full step-down feedrate and a field for minimum step-up feedrate, along with some simple math, should be enough to achieve what I am after. In my example I mention 1.0" deep at 400ipm. I would also like to have a field where I may enter 800ipm for the minimum depth cut. The computer should extrapolate feedrates for the cut depths in between based on the given values.

The depth and feedrate values I would expect to post are as follows:

Depth   -   IPM

1.000   -   400

0.950   -   421

0.900   -   442

0.850   -   463

0.800   -   484

0.750   -   505

0.700   -   526

0.650   -   547

0.600   -   568

0.550   -   589

0.500   -   611

0.450   -   632

0.400   -   653

0.350   -   674

0.300   -   695

0.250   -   716

0.200   -   737

0.150   -   758

0.100   -   779

0.050   -   800

In theory this should work well. There may even be a better method to calculate feedrates and having the option to choose would be nice. In the following you'll see that feedrate doubles at half the depth of the deepest cut until hitting a max feedrate.

Depth   -   IPM

1.000   -   400

0.950   -   440

0.900   -   480

0.850   -   520

0.800   -   560

0.750   -   600

0.700   -   640

0.650   -   680

0.600   -   720

0.550   -   760

0.500   -   800

0.450   -   833

0.400   -   833

0.350   -   833

0.300   -   833

0.250   -   833

0.200   -   833

0.150   -   833

0.100   -   833

0.050   -   833

I haven't machined anything with this exact method just yet, but I am eager to try now that I've taken the time to post here. I'll manually edit a roughing operation to do this then run it and post the results.

[Laurens-3DTechDraw]

Feedrate is actually more tight to the width of the cut and not the depth.

So if we would do that I would vote for it(And have in the past.)

But I see no way to change the feedrate based on the depth of cut if the width of cut stays the same.

[Tony]

Hi @avantmfg,

I think @Laurens-3DTechDraw is right, feed rate is more based on width not depth, it is common practice with solid carbide tools to cut as deep as the tool or job will allow use smaller step overs and feed at a faster chip per tooth, this allows for good & even use/wear of the cutters edges and also allows the cutting heat to be evacuated in the chip, also with higher feeds it helps fly the chip away from the job and cutter, if you were to use small depth of cuts with fast feed rates you would more than likely find the bottom and corner edges of the cutter to wear excessively and give you a poor finish.

It would also heavily add to cycle time in the machine, for example recently I machined a 500x500x50mm Square plate (20x20x2") and each corner of the plate was a different finished height, the only way to machine this was to run a parallel surfacing operation where the speeds were 8000rpm and 8000 mm/min (315IPM), I ran a 0.75mm (0.0295") step over and while it traveled the X axis it was also increasing and decreasing on the Z Axis, this took 50mins to machine each plate, this was resulting is approx 80-90% spindle load at the deepest point and 50-60% at the smallest, If i was to use your method above the tool feed would be slowing down and speeding up as it traveled along the X axis and that would then have added alot more machining time to the job.

I would be very interested in your results from your test of this method though. 🙂

[avantmfg]

@Anonymous-3DTechDraw and @Tony, I may not have articulated my idea very well. When I do the test I will make a video comparison of the toolpath as I use it now vs how I would like to use it, then I think it will be more clear what I am after.

[Tony]

@avantmfg sounds good, I look forward to seeing it 

[Laurens-3DTechDraw]

@avantmfg I really would like to see the video. Helping people make the move to HSM is always good 😉

[Rob.Lockwood]

again, it depends on what the limiting factor is.. If you're machining aluminum, and are being limited by horsepower during an initial roughing cut, then it's incredibly likely that feedrate can be increased when the cross section being cut decreases.

If you're cutting titanium, and you're being limited by the generation of heat caused by the action of cutting itself, then there are no gains to be found due to the decreased cross section, at least not in the ADOC direction.

As such, this is a complex problem that requires a far more complex formula than is initially apparent.

[Laurens-3DTechDraw]

@Rob.Lockwood While that is true, I believe for most people there would be more to gain in the width of cut optimisation than in the depth of cut/horsepower optimisation. But doing one might make easy work of the other.

[Steinwerks]

@avantmfg I too would like to see how this plays out. My experience tells me that it is not that simple. 

[highgforce]

I agree with you Laurens - change the width of the cut as the depth of the cut changes. In this way, the force on the tool can remain nearly constant. If you change the feed rates, the cut per tooth will change, and you could end up taking very big or very small cuts per tooth/flute.

[greg]

Not that I would run their garbage software, but isn't this the whole deal with iMachining?

[highgforce]

"Not that I would run their garbage software, but isn't this the whole deal with iMachining?" Yeah, I was initially trying to learn Solidcam, but all their different machining modules is confusing and ridiculous to say the least. So I gave up on that idea. They really need to simplify things to a certain degree. Adaptive Clearing, iMachining, Volumill, .... it's all the same concept. I'd like to see a side-by-side comparison and see which one works best overall. "As such, this is a complex problem that requires a far more complex formula than is initially apparent." It's complex, no doubt about that. Anyone want to take on this project for decade long, PhD thesis?

[Laurens-3DTechDraw]

@highgforce

I would say I take on the project but I would get bored. Because in the end being 95% right is all you are ever going to get.(If you can even get to 95%)

So no.

[highgforce]

For some material, tool, and other factors combinations, I suspect there would be a wide range of speeds and feeds to get you within 95% of the optimum. For other combinations, that range would be less.

[al.whatmough]

Batch processing ideas that are 10+ months old with less than 5 votes. This is in no way to suggest the idea isn't a good one. However, the lack of votes tends to mean that the community feels other ideas should be given a higher priority. Feel free to tag me if you feel an idea wasn't given enough of a chance. We are more than happy to have a conversation on any of these ideas.