Complex pocketing?

[dubstar-04]

I just had some time to look into the model.
There is no shortcut to this task.

In my opinion:
1. Face milling of each Drilled Post. With adequate positive "material allowance" value to make sure you make a nice platform there.

2. Drilling of each hole.

3.Then normal pocket milling of the bottom.

Why first facing: to produce a nice flat platform for drilling.
Why then drilling: because drilling on supported surface (not yet a milled post) is more rigid.
Why pocket milling at the end, so that the posts are generally shorter (so more rigid) and it makes clean cylinders.

There are no two ways about it, for some of this you'll have to use a small small tool.

----to note: it is completely wrong to call the option "material allowance" in the Face Milling tool, that is not how a facing operation works, most of the times you want to overshoot the whole face (fly cutter, large flat end-mills, clearing burrs...etc). So technically it should be "over shoot" by default or the adequate milling linguo for the overshooting. "Allowance" would only be true if using negative values of this parameters, that's when material is intentionally left untouched . Only in that case does "Allowance" make sence as a term. Perhaps a drop-down menu in the Face Milling tool saying "allowance" or "overshoot" with the editable value with only positive values accepted.

This seems sensible to me. I would probably use an adaptive roughing op to do the bulk of the clearing and then use profile operations to bring the part to final size.

AdaptiveClearing.png (44.86 KiB) Viewed 870 times

If you machine this part please can you post some photos?

Thanks,

Dan

[RatonLaveur]

Yes i agree. Step 3 in my original suggestion is best performed using adaptive followed by Step 4 profiling to accurately and nicely finish.

[toolmaker]

Thanks again everyone for all the help. I'll let you know if I get stuck -- if not, I'll be sure to post a pic of the finished part.

Best,
-Bill

[toolmaker]

I'm getting some nice results using multiple Pocket_3D operations.

Here's an intermediate result displayed in Camotics:

Intermediate result

CamoticsOutput1.png (95.69 KiB) Viewed 843 times

Quick question: Is there a way to force an operation to use the results of a previous operation as its starting point? (In other words, I want to keep operation #2 from milling areas that were already removed in operation #1).

Thanks!
-Bill

[dubstar-04]

I'm getting some nice results using multiple Pocket_3D operations.

Here's an intermediate result displayed in Camotics:

CamoticsOutput1.png

Quick question: Is there a way to force an operation to use the results of a previous operation as its starting point? (In other words, I want to keep operation #2 from milling areas that were already removed in operation #1).

Thanks!
-Bill

Unfortunately its not possible to reference previous operations results or do 'REST Machining' at the moment.

Thanks,

Dan

[toolmaker]

Ouch -- that hurts! I'm starting to understand some of the suggestions above (some of which seemed pretty involved). Is the limitation in the simulation? Has anyone tried using (manually operation-by-operation) Camotics to bridge that gap?

Thanks!
-Bill

[RatonLaveur]

At least in my case i can say that the simulation is only a check. I never use it as a way to optimize.

However you are right, the solution i presented was almost solely the result of having to do without rest machining.

[chrisb]

Has anyone tried using (manually operation-by-operation) Camotics to bridge that gap?

I don't think so. Such optimizations are currently mada manually by adjusting the depth parameters, and by using the profile operation which doesn't touch the innards of a pocket.