Most efficient strategy for milling many small features?

See attached screen shot of a sheet of parts I machine from .065" aluminum. I'm running the latest version of BobCAD/CAM. I have been struggling for over a year trying to learn to use it efficiently for my work and I'm giving it a heroic effort to break through a few remaining issues like this. I am very experienced with VCarvePro and for my 2-1/2D work it has been very useful and efficient. I am starting to get more into 3D so invested on BobCAD but have not been successful cutting parts until a month ago or so.

Attachment 314522

I need to rough out all of the small holes and shapes and then do a finish path on them. What is the most time efficient way - both time programming the CAM as well as machining time - to do this? I can imagine 2 strategies but perhaps there are others (particularly with the CAM):

1) machine each feature rough and finish passes one at a time. This is what I currently do in VCarvePro and it optimizes the finish pass so the tool is not extracted to start the finish pass (which is fill depth, material is .065" aluminum). Pros: seems to be the most time efficient, at least in VCarvePro, since extra retracts between rough and finish are eliminated. Cons: requires a lot of time to copy/paste the operation and then select new geometry.

2) machine all the features rough in 1 pass then go back and do the finish operation. Pros: minimal number of operations needed since all the geometry is selected at once. Cons: potentially takes longer to machine than 1 but I don't know this for sure.

I'd prefer to optimize for machining time since I make lots of these. I don't have the time to conduct experiments to see how these actually machine so I'm hoping someone here can help.

cheers,
Michael

I vote for strategy 2 just by gut but I can't say for sure by your description that I'm positive about what you are trying to do. Can you do a sample file with just a few parts (in BobCAD) so we can get an idea of how you go about it?

What I'm thinking is extruding all your geometry to create a solid, then use a 3D toolpath like Advanced Rough to handle the roughing. You would just need to select the outer circles as boundaries to confine the toolpath to the pockets.

Depending on how fine and accurate your finish needs to be a simple Rest Rough operation could do the finish work. Dirty? Yes. Fast? Yes.

I'll have to draw up some sample non-commercial parts to post. But...

I do have these defined as 3D solids in Rhino and I import the Rhino (3DM) file. That all works fine. I use 2 axis mill features for these as I have found that to be a lot faster. I use a pocket (inside to perimeter) as the roughing pass just to make sure the little cutout pieces don't cause problems. I learned this the hard way - these are cut with a 1/8" end mill and I broke a few of them when the little cutout parts stayed in the holes and bound the cutter. Once the "pocket" is cut, a profile pass at full depth does the finishing cut. I do need a finishing cut for both fit and finish.

Part of my challenge is not knowing what the heck all of those milling strategies mean. I can't find any definition/documentation for them. And when I did try to use Advanced Rough, once I configured it - probably incorrectly - the path was not actually created. I went back and tried a few other options but could never get it to generated code to create one of the pockets.

Give me 5 minutes and I'll have a simpler example to post.

Ok, I've attached a simpler version of the part with all of the cutouts in it. I would use a 1/8" end mill to machine these.

My original question was this:

1) is it faster to rough and finish each feature in sequence. The attached bbcd file (zipped) demonstrates what I mean by this. I would then copy and paste the Feature 2 Axis for each of the cutouts. With VCarvePro the tool can be configured not to retract after the roughing pass, it stays in the "pocket" and completes the finish pass. That same a lot of time when you are talking about 52 cutouts.

2) the alternative would be to do all the roughs first and then go back and do the finish. In this case, I would simply select all of the cutout geometries with the Feature 2 Axis and Compute all Toolpaths. It seems like there would be a lot of excess retractions that waste time.

I also have included my attempt to use the Advanced Rough as per your suggestion but as you can see, no tool paths are generated probably because I don't know how to use this feature.

Ahh, I see. Ok, do not select wireframe geometry for any 3D toolpath (except 3D engrave). Select surfaces or solids. In this example I just window selected the entire thing and hit recompute. Avoid using a stepover more than half the cutter diameter (0.0625 in this case) or you may get some strange looking results.

Try these settings in your Advanced Rough feature:

Parameters
Depth of Cut: 0.0325 (0.065/2)
Stepover: .0625 (no more than half the cutter diameter)
Top of Job: 0
Bottom of Job: -0.065 (this is an absolute value, not incremental like the 2D toolpath strategies)
Allowance: 0.015

Options
Make sure the sorting is done by Area, not Level (area is by default, if by level it will complete all cuts at the first depth then go back and do the profiles again at the second depth - more repositioning moves)

As far as which method is faster it sort of depends on a few things. Firstly, even with the 2 axis Pocket and Profile the tool is going to retract between each cut. There is no "keep Z down" option unless you script it like I did. Secondly, if your machine is relatively slow and you are a fast programmer you are always better off in 2D so you can control things like cut order a little easier. The 3 axis toolpaths make their own decision optimizing cut order and sometimes it's not all that optimized.

I still vote for the 3D method as I can extrude 2D geometry in no time flat and the 3 axis toolpaths take just a minute or so to setup. Here's a screenshot of what I did with your file in just a minute or 2:

Attachment 314544

This actually was my "Ahaa" moment when working with BobCAD. The hardest part was figuring out what type of geometry each toolpath wants. It lets you select geometry that it won't use, kinda goofy but you get used to it.

Oops, I posted the first screenshot I took, not the one with multiple depths:

Attachment 314546

I would post a file but I'm using Demo mode to play with your file.

Hey thanks! Some questions...

By "wireframe" do you mean the edges like I selected in my bbcd file as opposed to surfaces like you selected?

Also, it loos like you just do the advanced Rough with no finish pass?

Finally, you made the comment "unless you script it like I did" what did you mean by that? Sounds interesting!

Cheers,
Michael

Now, here's what a Rest Rough operation looks like:

Attachment 314548

The trick here is "lying" a bit to the toolpath. The Rest Rough won't allow you to use the same size tool that you initially roughed with, otherwise there would be nothing "rest" to remove which is logical. So I added 0.005" to the cutter diameter of the "Previous Tool Diameter". You must uncheck "Use previous operation" to do this unless you do the Rest Rough in an entirely different feature. No reason to do that as far as I can think of at the moment (unless you wanted to use different geometry to exclude something but even then you can have a separate boundary if you choose). See this screenshot:

Attachment 314554

If I'm way off base with what you're trying to achieve stop me now! Sometimes I overthink these things. Either way, this should give you a leg up on using 3 axis toolpath if you've not quite used them before.

Yes, this has been a good learning opportunity.

At the end of the day I'm just trying to figure out what operations and configuration is optimal for reducing milling time as much as possible. I understand very well how VCarvePro works so I naturally know which operations and how to configure them to do these things. I'm trying to develop that in BobCAD but it has been a much larger hill to climb due to all of the strategies and configurations.

thanks!

Quote:

---

Originally Posted by mhackney

Hey thanks! Some questions...

By "wireframe" do you mean the edges like I selected in my bbcd file as opposed to surfaces like you selected?

Also, it loos like you just do the advanced Rough with no finish pass?

Finally, you made the comment "unless you script it like I did" what did you mean by that? Sounds interesting!

Cheers,
Michael

---

Yes, that is exactly what I'm talking about, no edges for 3 axis toolpath. The edges work just fine for the boundary though as you have found.

No finish pass in the first Advanced Rough (allowance 0.015) but then I added a second Advanced Rough to do the "finish" pass using the Rest Rough option.

Scripting is a last resort. The "Keep Down Z" script took me 3 months to completely debug and I'm not sure it was worth the effort. There is an API for modifying the post output and you use VBScript to do things to your posted code automatically. I wrote a script to look for spots where the tool retracted and then went right back down in Z (no XY movement) and added a check mark to the feature to force the tool to stay down no matter what the next feature was (kinda dangerous). You can't simulate it either because it only appears in the posted code, not on the screen as toolpath. No collision checking, etc.

Quote:

---

Originally Posted by mhackney

Yes, this has been a good learning opportunity.

At the end of the day I'm just trying to figure out what operations and configuration is optimal for reducing milling time as much as possible. I understand very well how VCarvePro works so I naturally know which operations and how to configure them to do these things. I'm trying to develop that in BobCAD but it has been a much larger hill to climb due to all of the strategies and configurations.

thanks!

---

No problem at all. In the end you may go right back to the way you are doing it. The 2D strategies are easier to control and my machines are very quick (900-1200 IPM rapids) so I tend to be lazy on the toolpath and let the machine bang around and do it's thing. While it's running I'll be programming something else so it's just the way I work to be most efficient and less error prone (I noticed the profile in your 2 axis profile feature was cutting on the wrong side). The 3 axis toolpaths are definitely the lazy man's way of getting things done, lol.

Yeah, I still have to guess at which side a cut will occur on a profile. I did that quick and dirty and didn't simulate to see where the cut went.

Even with fast rapids, with this number of small features the time adds up!

Thanks a lot SBC Cycle. I've done a lot of work today and feel much more comfortable using the 3D tool paths for this type of work. I have something that looks good in simulation, minimal moves, etc. I need to finish the fixture for these parts (my old fixture is beat) and I'll try a few cuts. I'll start with a single part so I can compare speeds with 3 different strategies I used.

Awesome! Glad to help. I have done the same thing to save precious seconds that add up quickly when you are running large quantities of parts. It's well worth the effort!

Here's another thought - not a machining strategy+ though!

When we do small parts like this, we sometimes use double sticky carpet tape to hold them down. Clean the surface, tape down, place the part. It has been very effective for us, and cleanup is easy (acetone or laquar thinner do a nice job). It will hold the pieces in the center as cut outs and keep them from getting sucked in to the cutter.

Another tack is to use supper glue - however, it is harder to clean up. We use it a lot for fixturing. If you can heat the parts to 400°, they come off easily as that breaks the bond.