Island Boundary question

I'm using V26 and doing mostly 2D, but definitely some 3D toolpaths. I've attached an example of a part where I'd really like to toolpath just the ring, but when I select inner and outer boundaries, it still calculates the toolpath across the entire middle surface. I use mostly planar and z-level finishing, as equidistant usually chokes my machine. The boundary issue only seems to manifest itself on finishing toolpaths - the roughing algorithms calculate as I'd expect.

I've tried selecting just the 'bottom' surfaces as machining faces, and tried selecting ALL, and using boundaries to limit the toolpath. It doesn't seem to make a difference.

Can anyone either shed some light on this workflow, or point me in another direction to do accomplish the goal?

I've attached one sample part, and one real one for kicks. Any help appreciated.
Todd

What strategies do you have available? Do you have Mill Standard or Mill Pro?

Nevermind, I see you must have Mill Pro if you have equidistant. There are really two options in my opinion. First, you can use equidistant, which is really the ideal toolpath for the job. From the sounds of it, your computer gives you trouble with that, but it would be the ideal solution. In V26, you would also want to offset a boundary inward from the perimeter of the outside of the machining area by half the tool diameter. The reason for this is that the tool will go to the boundary at the centerline of the tool, not the outside of the tool, which means that it will start at the surface and step over and slightly downward while running along that outside edge until it gets to where you could have put the boundary. If you just put the boundary half the tool diameter inside of the region you want machined, you'll skip a lot of unnecessary cutting. In V27, they added some features to Equidistant Offset that are invaluable, one of them being that you can just set the toolpath to be "inside" the boundary, as opposed to "centered" on the boundary. You also have the option of setting the tool to go completely outside of the boundary for those situations where you need some overlap. V27 eliminates the need to create wireframe boundary geometry where I used to have to generate it 90% of the time. V27 also added "Spiral" as an option in place of a zig zag or zig motion around the part. For this particular file, the spiral is probably the most ideal as it will just run around the part in circles until the whole region is cut, with a couple areas that at each corner that get a little extra help. If the inside and outside boundaries were completely offset (as in the outside boundary had radius corners that keep the channel to a even spacing all the way around), you could even use drive curves and it would run in perfect rings around the part, another control added in V27. In V26, you can get a pretty decent toolpath just with extracting the outer edge geometry and then offsetting it in by half the cutter diameter.

The other approach would be to do it in 2 planar slice sections (as subcategories of the feature you have). In this approach, you could use parallel cuts (Planar Slice), and boundary off each side of the rectangle. You then set the direction of the cut to run parallel to the each channel. This would be easier on your computer than Equidistant offset, but would require a little more work in programming. Still, it should be pretty manageable. Again, I'd offset the outer edges in by half the cutter diameter, but keep the inner edges as they are. You'll also need to create another boundary for the inner corners since this would not allow you to get into those, but that shouldn't take too much. Something to note is that you can create individual boundaries for each portion of the feature by leaving the feature level boundary blank. Under each sub-category (Z-Level, Planar, etc.), you can create a boundary just for that function. I've attached a quick file showing this method, but it's not really done. I think you'll get the idea from there.

Another quick note, generally I just select all the solid geometry and use boundaries from there. I reselected the geometry in your file to include the entire solid on that layer. I see there are other layers inactive, so I left those alone. Picking individual surfaces often leads to trouble since the boundaries of the machining area are not as well defined. At the very least, you need to pick the bottom surface, the vertical walls and a top surface surrounding that region or it may gouge the part.

Thanks a ton, mmoe -

I had experimented with the segmented-boundary approach as you described, and it works well enough. As you say, a bit more programming, but it works.

So the second part of the workflow question (maybe I should start a new thread?) is that - as you saw - there are often lots of layers to these parts. My workflow is...... workable, but maybe a bit clumsy. These parts are often 1-off molds made of MDF for fiberglass layups. So far, I've been using 3/4" MDF, and sticking to short Onsrud cutters.... often a 3/16" ballnose EM for finishing. I then laminate all the layers into a big mold for layup. It requires a bit of bondo & sanding before layup. My router has a 4" height restriction. I sometimes laminate stock up before machining, where geometry allows it. I have some longer cutters ordered up, just to see how they work in MDF. I think they'd work great in foam.... skeptical (but hopeful) that they'll work in wood. Most of the parts have 8-12 layers.

So the workflow goes like this:

Client sends me a STEP file.
I pull it into Inventor, and slice up the solid into 3/4" layers, and export as IGES.
Import IGES into BobCAD, and create separate layers for each slice, and UCS's for the top & bottom of each.
Create a new milling job for each layer/slice. Run Stock wizard and set the Stock to layer extents, with machine setup pegged to the corner of the stock.
Then I work through each layer, extracting top and bottom edges... offsetting, running my Z-level rough / finish. Lather, Rinse, Repeat.

This is just MDF. We fill & sand to get fair curves... I probably don't need tolerances much better than .030", but a smooth finish does help.
I agree - equidistant is what I should be running. I use it on simple things... but it often chokes when I give it something more complicated to chew on. (Yes, new workstation is the 2015 budget)

I just wonder if there's a simpler approach to doing the layered thing. I tried creating all the milling features in a single Milling job, and setting top and bottom of job. I run into problems with height restrictions on the machine.... I can't re-zero out that high, etc.

Any thoughts would be most appreciated. I may have learned something re: offsetting boundaries - I had been offsetting them OUT to allow the tooltip to get to the top of the geometry, but the way I'm hearing from you.... I should be offsetting IN to prevent the tooltip from riding up and over the edge? I tried it that way, and it doesn't seem to make a difference. I might just be looking at the limitation of planar strategy, though. It's probably doing exactly what it's supposed to do.

Thanks!

I think I'd slice it up as you are doing. You could do it off the full solid, but I think there are some key functions provided by slicing it that are hard to pass up, such as providing edges to use for establishing boundaries where the areas are ramping down to the bottom of the material. You don't really need to create a UCS for each layer though. You can just select the machine setup origin off of the part geometry so long as you orientate it on the X and Y plane correctly to start with. The part as it was in your file is rotated, so you need UCS's to make that work. Rotate all the geometry and you can just click the "Origin" button in the setup and then click on a corner of the geometry (does not have to be the stock geometry, can be a snap on the model geometry). You can then call the top of that setup "0" and then define the bottom of the job while also selecting only the solid for that layer of MDF.

Thanks again, mmoe.

I'd toyed around with the idea of reorienting geometry, but didn't recognize that it would make the UCS part simpler. Given that, it makes much more sense.
I'll revise the workflow and hopefully some longer tooling will help as well. (Not that I really look forward to moving >1" MDF around the shop)

Just a thought,maybe make each slice/layer a different color also.Might visually help keep it orderly ???????????