Help with Skateboard Model

[Carlson]

So after running a 3D probe on a skateboard for 50 hours the result was a pretty darn clean model. Through the 'Copy Machine' I saved it as a .SBP and then using the 'Surface to Probe' function saved it was a DXF Surface and brought the resulting file into Aspire 4.0 (as learned from Brady W.). Once I set up job size and import the 3D model everything looks good. When I zoom in however the edges of the skateboard that should be perfectly smooth have little ridges along them (assuming from the raster pattern the probe uses coupled with the .03" step-over). Some areas are more prominent than others (see attached 2 photos). Is there a way to smooth these out other than the 'Sculpting' tool in Aspire? Or will these small ridges affect the profile cut at all?

The purpose of this model, once edges are cleaned up, is to use it to create molds for our hydraulic skateboard press, use the profile shape of it to cut out the board once it is pressed, and to use the hole placement to properly and accurately drill the 8 holes in each skateboard. The boards are made by applying glue to 7 plys of sugar maple veneer that are 9.5"x34" and putting them in the press with the shaped mold inside for 1 hour. Once removed from the press we are left with a pressed rectangle (see attached 'blank side view' & 'drilled blank'). This is where we need to make a profile cut that is the shape of the outer boundary dimensions of the 3D model cut into the center of the rectangle (pill shape)(see attached 'blank and cut'). After we create a vector boundary in Aspire and apply a Profile Toolpath it only allows 2D so the spindle can't raise and lower when it's at the nose and tail of the pressed skateboard. Air cutting the file it does in fact show it only will do the pill shape without raising/lowering at the nose and tail. What would be the easiest way to accomplish this cut out? This will be repeated time and time again once we get it dialed in. The drill holes we are not worried about and that will come after we figure out this issue with the profile cut outs.

For the mold making part we will be able to create a toolpath that replicates the probed surface and mill out a rectangular block of laminated hardwood with the resulting toolpath. That will actually create the bottom piece of the mold for the press. Probing the bottom of the board will then give us the top part of the mold. Shouldn't be too complicated, we should then be able to scale the model up and down in Aspire to create different sized boards with the same dimensions.

Bottom line questions:
1) How to I smooth out the outer perimeter of the skateboard file that was probed?
2) How do I cut the "pill shape"(centered) out of the pressed board rectangle? (pressed board rectangle= 9.5"x34")(pill shape= 8"x32")

Thanks in advance guys, sorry for all the reading figured I would be as thorough as possible.

[Carlson]

This is exactly what I need to do. CLICK HERE FOR VIDEO

[Sk8MFG]

It is a fairly simple process, looks like you've taken the scenic route.

This is how I do a mould and toolpath in about ten minutes.

1. Fire up Illustrator and create the outline cut, and truck hole vectors.
2. Create a vector to represent the concave of the board. Create another to represent the profile.
3. Import the concave and profile vectors into a CAD program. Rail extrude to create the mould surface. Tweak as necessary. Offset surface to give correct mould offset, dependent on the number and thickness of blanks you will press per mould.
4. Import male and female mould surfaces to Aspire.
5. Create toolpaths to cut the mould.
6. Create a cut file in Aspire using the female mould surface (assuming you are cutting bottom up)
7. Import outline and truck hole vectors. Create drill toolpath, create outline toolpath projected to surface.



One more point. If you're doing 4 or 5 decks per pressing, you may have to modify your cut routine to match the projected surface to the "real" surface of the deck. Since each blank will have a slightly different concave, a tool path for the bottom blank may not work for the top one. Especially important if you are using a compression bit (best choice).

[waynelocke]

You probably need Aspire for the toolpath. It has a "Project toolpath onto component", This will raise the spindle like the video.

[Carlson]

It is a fairly simple process, looks like you've taken the scenic route.

This is how I do a mould and toolpath in about ten minutes.

1. Fire up Illustrator and create the outline cut, and truck hole vectors.
2. Create a vector to represent the concave of the board. Create another to represent the profile.
3. Import the concave and profile vectors into a CAD program. Rail extrude to create the mould surface. Tweak as necessary. Offset surface to give correct mould offset, dependent on the number and thickness of blanks you will press per mould.
4. Import male and female mould surfaces to Aspire.
5. Create toolpaths to cut the mould.
6. Create a cut file in Aspire using the female mould surface (assuming you are cutting bottom up)
7. Import outline and truck hole vectors. Create drill toolpath, create outline toolpath projected to surface.



One more point. If you're doing 4 or 5 decks per pressing, you may have to modify your cut routine to match the projected surface to the "real" surface of the deck. Since each blank will have a slightly different concave, a tool path for the bottom blank may not work for the top one. Especially important if you are using a compression bit (best choice).

Thanks Sk8MFG, I completely understand creating a board from scratch in Illustrator and have already played around with it. We decided to do this board because our team skaters love the shape/concave and we want to replicate a mold for it, which is easy and we've already got it started. I realized what I was doing wrong and now have a clean profile cut that goes up and down at the nose and tail. We are cutting face up and are dialing in the spoilboard template we will be using specifically for boards. Curious as to what bit you use and the diameter you drill your truck mounting holes? Also is there a specific compression bit you could recommend for cutting out decks? As well as recommended feed speeds/RPMs? That would make a WORLD of difference We are doing one deck at a time, no stacking and cutting. Just traditional 7-ply Great Lakes Sugar Maple veneer glued and pressed. I greatly appreciate all your help Sk8MFG.

You probably need Aspire for the toolpath. It has a "Project toolpath onto component", This will raise the spindle like the video.

Thanks for the response also waynelocke, I was doing that in Aspire but didn't have it set properly and the toolpath wasn't on the model, it was going right around the outside edge, hence it not going up and down, it was doing a 2D profile. Changing the cut to "Inside/Left" of my boundary vector made all the difference, one click

[Mayo]

I'm curious what is the advantage or reason why you want to cut it after it's molded?

Can you cut your individual plys before glue up and pressing in the molds?

Or glue up the ply flat, when dry cut it to shape, then press it.

Is it a problem trying to press it after the glue has cured?

[Carlson]

I'm curious what is the advantage or reason why you want to cut it after it's molded?

Can you cut your individual plys before glue up and pressing in the molds?

Or glue up the ply flat, when dry cut it to shape, then press it.

Is it a problem trying to press it after the glue has cured?

It isn't possible to press the boards a second time to give it the concave/kick shape it needs, once the glue has cured after they are pressed initially, that's how it's staying. Each of the (7) 9.5" x 34" plys of veneer are glued and put in the press to get their final concave/kick shaping, after that we then cut out the pill/popsicle shape with the CNC and drill the 8 mounting holes for the trucks and then hand finish the edges. Basically the SOP, expect a lot of small/medium (even some large) companies use band saws and shaper tables instead of CNCs, but we want to be on point and be able to do custom molds for our press.

Thanks for the show of interest Mayo, skateboards are function works of wood art.

[Sk8MFG]

Thanks Sk8MFG, I completely understand creating a board from scratch in Illustrator and have already played around with it. We decided to do this board because our team skaters love the shape/concave and we want to replicate a mold for it, which is easy and we've already got it started. I realized what I was doing wrong and now have a clean profile cut that goes up and down at the nose and tail. We are cutting face up and are dialing in the spoilboard template we will be using specifically for boards. Curious as to what bit you use and the diameter you drill your truck mounting holes? Also is there a specific compression bit you could recommend for cutting out decks? As well as recommended feed speeds/RPMs? That would make a WORLD of difference We are doing one deck at a time, no stacking and cutting. Just traditional 7-ply Great Lakes Sugar Maple veneer glued and pressed. I greatly appreciate all your help Sk8MFG.

If I understand correctly, you've simply set the toolpath to cut on the inside of your outline vector and then projected that to the board surface? I think you'll end up with some problems doing that. Specifically, by cutting on the inside of the outline you will end up with a board smaller than the original outline.
To cut a board to spec per the outline, you need to cut on the outside of the path.

One other major issue you will run into is re-creating the mould. You won't be able to extrapolate the space between the scanned portion and the edges of the mould with aspire. You also will not be able to do the surface offsets required for the male and female moulds, they are not identical.

We use a 1/2" single flute compression bit at 6-8IPS depending on material and construction. Your feeds and speeds will be dictated by the bit. 3/16" boring bit for holes.

[Carlson]

If I understand correctly, you've simply set the toolpath to cut on the inside of your outline vector and then projected that to the board surface? I think you'll end up with some problems doing that. Specifically, by cutting on the inside of the outline you will end up with a board smaller than the original outline.
To cut a board to spec per the outline, you need to cut on the outside of the path.

One other major issue you will run into is re-creating the mould. You won't be able to extrapolate the space between the scanned portion and the edges of the mould with aspire. You also will not be able to do the surface offsets required for the male and female moulds, they are not identical.

We use a 1/2" single flute compression bit at 6-8IPS depending on material and construction. Your feeds and speeds will be dictated by the bit. 3/16" boring bit for holes.

Thanks again Sk8MFG, I was trying to get the process dialed, not actually cutting any pressed blanks off that model. I understand cutting on or inside the vector and how it affects size, again it is just for learning purposes right now on my end. I have a buddy who has worked on CNCs and 3D modeling software for over 15 years and he's doing all the molds for us with his software. He's just on a month long trip in Japan so I am just seeing what I can do with my new toys. I have a pressed uncut I probably should have scanned instead if I wanted to "attempt" a mold myself. Curious as to how you adjust the kick at the tail/nose just before they rise when you make the mold in Illustrator? I understand building the concave, just can't grasp the kick...

Offset! How is the offset calculated? Is that just the "thickness" of each deck? That is actually something I was real curious about but couldn't find answers/info anywhere.

Thanks for the bit info also, I get how each bit requires different feeds & speeds and for different material, I was just curious what type of compression bit you used to eliminate trial-and-error for figuring out shank and flute numbers. Also didn't think too many guys on here use their machine to cut laminated veneers, 7-ply especially. We've been drilling 3/16th for mounting holes so I figured the same but wanted reassurance, the CNC has made things much different. And for making molds, a first also.

Thank you so much Sk8MFG, I hope to repay you in someway for saving me time and headaches.

o/-<|:

p.s. Misspoke in original post, the purpose of the model wasn't for recreating the mould in Aspire. Sloppy choice of words.

[Sk8MFG]

Sounds like you've figured most things out. Your friend shouldn't have much trouble building the mould surfaces. He should know how to do offsets without issue.
Adjusting the surface is easy in a CAD package, rhino, autocad etc... There are a few different methods. One is to create two "concave" vectors in illustrator. One is the real concave, the other is simply a straight line. By importing both you can use the profile vector as a guide. Place the concave vectors in the middle where you want concave, use the straight lines at the transition from deck to kick. Once everything is in place, you can loft the concave lines together to create the surface. The straight lines will remove the concave at the transition and up the tails. It will take some time to tweak as some programs make a "best fit" when it comes to loft.
Bottom line, use CAD for any and all actual 3d work. Aspire for generating tool paths.

The offset is very important for a solid lamination. The male/female offset is the thickness of the blank. ie. a 7 ply would be a 0.4375", two blanks would be 0.875".
We run our face veneer through our thickness sander to save on labor. The sanded faces are thinner than the raw veneer, that difference should be taken into consideration. Your buddy will know how to do it.

As for feeds and speeds, we cut everything from 3 ply with carbon and basalt to 10ply with fiberglass, or raw wood. Each requires a different speed and feed. The composite decks require a slow speed and feed, all wood higher. The bit manufacturer should have a table which indicates the best chip load for the bit you are using. There are some calculators out there which make it easy to determine what feed and speed you need to match the chip load (how much it actually bites off per revolution).
The chip load is a great base line. We have a big Alpha which has been modded a bit and a very strong hold down, we can really turn up the the speeds putting us above the recommended chip load. This causes more wear on the bit, but when we are doing a several hundred board run every second helps. It will take some trial and error for you to figure out what works best.

For the holes, we use a 3/16 boring bit. Not a brad point, or regular twist drill. We found brad points and twist drill bits have far too much blow out. The boring bits are often used for doing holes for the small pegs for closet shelves.
Depending on your finishing, you may need to step up to a 13/64". Clear coat can cause the 3/16" to tighten up a bit too much and chasing the holes by hand is a pain.

If you want to repay me, let me build all your decks
Always have capacity for more projects.... but then again, you did just get yourself a fancy toy.