3d Adaptive ignoring rest machining request?

[davek0974]

I have a simple test project that is not going how i wanted

It has three cam processes - a 1st pass with a large tool to clear away bulk, then a second pass with an intermediate tool using rest machining to clear the corners left by 1st pass, then a final pass with a small tool to clean up the waste left by tool 2.

The last pass however is ignoring my request for rest machining and doing the whole surface, which even on a small part with a 1.5mm tool takes hours and is a total waste.

Any reason it would ignore rest machining??

I dont know how to share the project but if someone lets me know i will do it if it helps Happy I did get a project link - maybe thats all thats needed?
A360

Thanks

Similar Threads:

• rest machining
• Need Help!- Rest Machining
• Rest machining is cool, but what is it doing?
• Rest machining
• rest machining

[precisionmetal]

I looked at your project.

I too have had problems when trying to do multiple (more than 2) sequential machining processes while using "Rest Machining".

For starters, I believe you'll want to change your strategy away from "Adaptive" on your last operation. What I would do is simply machine the profiles, with maybe one or two roughing passes.

PM


Here you go.... try this ---> https://www.dropbox.com/s/x70us6qmz5...8b%29.f3d?dl=0

[davek0974]

Thanks for that.

I had it working yesterday on another test file, it had four tool passes, the last three were all rest machined and worked. Seems a bit random to me, rest machining also has all those tiny wasted moves - there should be a way of filtering them out.

I never looked at rest or 3d adaptive until this week, they are much faster which matters with small tools as the parts take hours otherwise.

[precisionmetal]

I've gotten away from using Rest Machining very often. After chasing things a bit like you are doing, I typically try to do one adaptive machining run, and then I use pockets or contours to do the rest.

PM

[davek0974]

Hmm, i have a lot to learn it seems.

The only thing i'm concerned about with it not being rest machined is that with the 1.5mm tool doing the cleanup, its going to plough into some solid areas in the internal corners of things like the "M" - possible tool breakage.

[precisionmetal]

Check out the quick path I made -- I just did a couple of roughing passes with 1/2 diameter stepover.

Sometimes it's faster to just make a very quick tool path in CAM, be generous on "safety" space, and get the machine going.

Spending a lot of time fine-tuning the tool path is great if you're going to be doing production, but for one or two parts I don't mind having the tool cut air for a bit in exchange for not wasting much time on the CAM.


Just my approach....

PM

[davek0974]

Good point, i was sliding into the "perfect path" trap i think

I'll get that test on the mill this week, its just a trial for some larger signs i want to make.

[precisionmetal]

It's easy to fall into that trap believe me.

It's fun to try and get the *perfect* tool path, but after finding myself spending 30 minutes tweaking a tool path and then realizing the part only takes 5 minutes to machine...

Eventually came to the conclusion that sometimes it just pays to get the part done quickly. I'm with you though: sloppy tool paths always bother me, even if the part turns out fine!

PM

[davek0974]

Looking through the post-code, it looks like the Z heights are messed up but cant see why, this is from the file header...

(T80 D=5.556 CR=0. - ZMIN=-1.99 - FLAT END MILL)
(T81 D=3. CR=0. - ZMIN=-1.6 - FLAT END MILL)
(T82 D=1.5 CR=0. - ZMIN=-2. - FLAT END MILL)

Now, all Z heights should be -2.00mm as they are all from the same model, no axial stock-to-leave is used on any path. Clearly this will make a mess on the last path due to slotting cuts plus the second pass is not as deep as the first??

Have i missed something ???

[precisionmetal]

I just looked at your original model:

op #1 -- you selected selected "Stock Contour" in second tab. This is wrong. Uncheck that box and select your geometry in the "Geometry" section immediately above it. "Stock Contours" is not for the purpose you chose.

op #2 -- you chose no Machining Boundaries in this same window/tab

op #3 -- you chose no Machining Boundaries in this same window/tab

[precisionmetal]

Here you go -- take a look at this. Note the "Geometry" I selected for the tool paths.

https://www.dropbox.com/s/4ei6mmvrsb...%20v3.f3d?dl=0

PM

[daniellyall]

I answered your post on the fusion forum torences and smoothing .001 and 0.0001 fixies the problem

[davek0974]

I answered your post on the fusion forum torences and smoothing .001 and 0.0001 fixies the problem

nope, sorry, it pushes the first op to -1.995 but not -2 and the second op is still -1.6

I'm going to have a look at the file posted by precisionmetal below.

[daniellyall]

Change the Adjustment to as computed and the Adjustment offset to 0 and the fine stepdown to 1 instead of .8 on the second toolpath the 3rd change the Adjustment to as computed and the Adjustment offset to 0 .995 is just outside nasa specks

[davek0974]

Thanks, that's getting there although i need to read up on what all these settings do.

It's not the precision that matters at all, it's the fact that i asked for -2.00 and it could only go to -1.995 and not 2. Where did it loose the 0.005mm?

[daniellyall]

You would have to ask the dev guys that question

[davek0974]

You would have to ask the dev guys that question

I guess so, its not that important though.

One way to fix it i just noticed is to select the TOP outline of the model and then set bottom cut height = "Stock Top" -2.00 that works ok so it must be an extrusion thing causing the 0.005 loss?

[daniellyall]

That's just one of the many ways to do it, how you had it for a start but with stock contour ticked is a way that works as well, there's a lot of different things that can be done for an adaptive toolpath to work or not work. and the rest machining if you have it as, as computed with offset of 0 it works better.

[davek0974]

Many thanks

[davek0974]

While on this topic, when rest machining following a roughing pass, is there an adjustment or setting to stop the tool trimming the microscopic bits left from before on things like curves??

It really only needs to go into corners etc where there is real material to remove, instead it wastes time going over tiny detail that a finish pass will easily fix.