Toolpathing in Aspire, the l-o-o-o-ng hard way!

First off, I hope everyone had an amazing holiday season, and Jody and I truly hope that the arrival of 2015 brings amazing things for everyone!!

We had a few NDA projects over the holidays, and a couple that weren't. So I thought I would get started with the couple that we're allowed to share.

The first one was what should have been a simple one, but progressively took more time than I had planned on. Hey, it can happen!

A neighbor a few units down from us does major renovations, for some pretty big custom properties.
He had contacted us in hopes that we could match his custom trim profiles for a series of arched top windows in a huge house he was building.

"Sure, should be pretty quick" I thought out-loud...............

I took his trim profile, traced it onto a sheet of paper, and scanned it into the computer, and adjusted it for some minor differences. This clearly would be made from 2 pieces, as the machined out waste would be way too much!

I tackled this this project in the usual way. I swept my profile along the 2 rails that match the window opening, then set up a 3d offset machining strategy, so the cutter would machine along the length of the trim, hopefully giving me a wonderful piece of custom trim, that will match exactly to all the other trim that already exists.

 Here's where it pretty much fell apart for me!

Due to the X and Y size of the window trim, versus it's relative skinny width, versus the resolution of Aspire on an entire 4X8 sheet of MDF, it didn't come out very well. On a 4X8 sheet, with the maximum 50X resolution (the highest Aspire reaches) it put a voxel pixel at around 1/16th of an inch. So couple that, with a .125" cutter, and you get a relatively rough piece of trim. Add to that, the long 3d machine time of multiple pieces of trim, and it all boils down to finding a better way to deal with this. The estimated machine time, including cutter changes, was 6 hours a sheet. PFFF.......

Aint nobody got tahm for dat!

So I was forced to re-think the process. I decided to go with many, many, many, single profile toolpaths, at the varying heights required.

So the above image was my self-torture test. Each circle represents the .125" ballnose cutter, and the vertical lines are the .025" stepover. These were originally laid out in Corel, as I still find I'm faster at some portions of vector work in it. But the actual offsetting of the vectors for the all the trim profiles, was done in Aspire, because that portion was faster in it.

This was the vector-jenga-mess I ended up with! Then it was just a matter of assigning each vector to a separate profiling toolpath, with the cut depths based of the first image above. The good news is I was able to re-purpose all the toolpaths for each successive piece of trim. Then I just saved all 27 profile cuts, for each piece, to one toolpath file.

WAAAY more computer time than I had first anticipated, but it got the machine time down to 45 minutes a sheet, and the trim was flawless!

8)
JWO

Machining The Second Layer!

With the second layer component now visible, and selected in the working window,

I used the create vector boundary tool, then offset the vector outwards by the same .300" offset.
In cases like this, I would toolpath this vector before-hand, and have our Techno cut the flat shape, having it on standby for gluing on. Or, you could just cut a rough block of  1" at this point on the saw.

We're going to assume I've now glued the second layer of material to the first layer that has already been machined.

The next step is to draw a box around the entire object. We'll use this to create a "false bottom"

Using the new box vectors, I set the height of this new component to 1.7" inches. This is approximately .250" below the actual surface of our real world material block on the cnc.
Make sure to set it to "MERGE"
The reason I do this, is to completely remove the danger of the cutter wanting to plunge all the way to the table surface, where the geometry of the model permits. Largely between the leg area. Without this block, I would crash the collet into the model, due to the shorter tool length were using.

You can see in this image where the seam is, and that the tool will completely machine over it, but just down to the block component.

Now we can turn on the second layer slice, and get ready to toolpath!

We now have to adjust our material setting. The first layer block was 2", we then glued a 1" block to our first slice, so the new material thickness becomes 3" total. Make sure you leave the Z zero at the bottom still.

With our 2nd layer offset vectors selected, I simply calculate a new roughing and finishing pass.
This machines the second layer, and removes any of the glue that may have oozed out during laminating the 2 layers. Keep in mind, the glue has to be dry. Usually we use a CA clue with HDU, so the dry time is pretty fast!

You can do this indefinitely,  adding layer by layer. Without having to buy longer and longer cutters, or machine separate slices, and glue them up, trying your best to line them up together.
I do this all the time, and it certainly saves a lot of post finishing. Just be sure to adjust your material block height in the setup window for each layer.

Not rocket science, and I'm sure I'm not the only one doing it this way,
but hopefully it might help someone who hasn't done it before!
8)
JWO

Slicing Made Easy!

Since we finished the butterflies, we have been busy making a couple of video game characters for an exciting new game! These guys are full size at 78" tall and made almost entirely from HDU! I can't post anything else about it until the NDA is up in March, but I have been documenting it as I go.
We also have some pretty cool film props that also have an NDA, so I'll post them later as well.

In the mean time, I thought I would do a helpful post on slicing 3d models, and getting the cnc to clean up the glue joints.

There are a million reasons why you would want to slice some model parts on the router.
One of the biggest for us, is that we are sometimes limited by available cutter lengths or material thicknesses.
For example, when were cutting a model over 3.5" thick, but the available material only comes in 2".

One way is to have Aspire slice the model, machine the parts separately, then glue them up. But then the seams require work to clean-up after. I much prefer letting our Techno do as much work as possible, because it does it faster and better than I ever could!

So here's a 3d model replica I made of the Excel gum's bad breath coffee guy like in their commercials.

As you can see, the front half of the model come in at 2.4998" thick on the Z axis. The problem is my
HDU material is exactly 2" thick. I also have a piece of 1" material I can use as well. I could glue them together into a 3" thick slab, but the other problem I have is that my 1/4" ballnose cutter is only 2.5" long. So after it's slid into the collet, I only have a total of 2" of cutter length available! I certainly can't do it all in one shot...........or can I? (dun, dun, dun) That was cliffhanger music you just hummed..............

First thing up is to slice the model into layers I can use.

In order to overcome any material variances, I slice my model just a hair under the material thickness. In this case 1.95". This will let the cnc plane off .05" creating a dead flat surface to glue the 2nd layer of the model to.

Here's our model, sliced at 1.95" thick, and the second layer turned off in Aspire.

I had Aspire create a vector boundary around the whole 3d model slice, then offset it outwards just over the .250" ballnose diameter we'll be cutting this with. In this case, .300" This will limit the toolpath so we don't machine the whole 12" material block.

At this point, it is important to add some small tabs to hold the model in place for the second layer machining. I simply drew some rectangles, and made the .250" thick. Make sure to set the tabs to "MERGE" or they'll pop out the model, looking weird. This should hold it while it cuts.

When we set-up our material block in Aspire, we want to set the Z zero to the machine bed/ bottom of the material block. It get's to be too much of a math game for me to set it to the top of the block :)

So this is the roughing pass done with a .250" ballnose cutter. I'm a little lazy, so I usually rough and finish with the same size cutter to eliminate a manual toolchange.

And the finishing path as well! As long as you don't do a cutter change between the roughing and finishing pass, you can use the same vector boundary for the finish machining. Aspire calculates differently between an endmill or a ballnose, A ballnose gets calculated to the centre of the cutter, while an endmill calculates to the edge of the cutter. So if you plan on using different cutters, you'll have to adjust the vector boundary accordingly.

Tomorrow I'll cover the rest of the process...........
8)
JWO