How do I split parts with an imported 3D surface?

[Zweerink]

I'm designing some oddly shaped strips of plywood that are too big to fit in my CNC, so I am cutting them in sections and gluing them together with a fingered lap joint.  My plan was to model the whole piece and then use the split command to divide them into separate solid bodies.  I have designed the fingered lap joint, and I used the thicken command with an offset of zero to make a surface of it, then exported it, then made a derived part that contained just that surface.  Now I'm stuck.  

How do I output that surface to a file that I can import into a part file?

[cadman777]

If I understand your goal, then you don't 'output that surface'. Instead, you do this:

After you make your original part (you don't have to do all the stuff that makes a surface), you make a new part, then DERIVE the original part into the new part. You can set the Derive options so the Derived part is a surface, then you can delete faces off that surface to get the geometry you want.

I'm not really sure exactly what you're trying to ultimately accomplish, b/c when you said you divide it into separate parts, are you talking about splitting it up the middle lengthwise or widthwise?

How is the board not fitting into your CNC router?

Which dimensions are too big?

There may be other ways to do it that are easier...

[Frederick_Law]

Derive and substract.

Cut the solid piece short.  So it keep the fingers.

Put a long rectangle piece and the fingers in an assembly.

Assembly the finger on the long piece.

Derive assembly into part and substract the finger.

You can assembly finger on both ends.

You can setup the "length" of the finger piece so you can easily get correct length from the long piece after subtraction.

[Zweerink]

My CNC router is 4 feet x 8 feet, and that's how big my plywood is too.  I'm cutting some odd strips of plywood that are 6 inches wide, but like 12 feet long.  I want to make the piece a single part, then split it into three sections that are 6 inches wide by about 4 feet long.  The fingered lap joints are super complicated to model, and really difficult to place as an ifeature on these parts.  Splitting my part along the glue line would be a super easy way to make two parts that fit exactly as they're supposed to.

You can split a part into two solid bodies with a surface, then derive the solid bodies into their own parts.  I've seen videos on it.  I just can't figure out how to get a surface into a part when the surface isn't a simple extrusion of a line, but rather a 3D shape.  I've seen videos of people projecting surfaces or cutting objects with complicated imported surfaces, but I can't figure out how to make an importable surface file, how to import it, or once it's in a part, how to place it since there are no constraints available in the ipt environment.  

Here's how the actual parts look when cut (this is just a test piece):

[Zweerink]

Your idea was generally what I was doing at first, but I have hundreds of these parts to do, and they're all different.  Every strip of plywood is a different shape, and many of them don't even have constant radii on the curves, and it is critical that the joined sections combine to be exactly like the piece before it's divided into sections.  If I could just plop a 3D surface into a part like it was an iFeature that would be ideal, but I can't figure out how to do that.

[cadman777]

OK, so let me get this straight:
1. your 8' long sheet of plywood isn't long enough, so you want elongate it.

2. you want to make a glued finger joint that's an overlap joint to do that elongation.

3. that means your router table mills down the plywood's face to 1/2 it's thickness, and also cuts the finger joints on the end and where the mill-down edge is in the middle of the sheet (that's your glued joint).

4. you want to make 3 parts that are 6" wide and join end-to-end to total 12' long.

5. both ends are identical, having a finger joint on only one end, and a chop cut on the other.

6. the middle part has finger joints on both ends.

7. you want all 3 parts to be the same length (4').

8. you want to cut all these out of full sheets of plywood, that is, you don't want to waste plywood, except for a 1/8" saw cut where the parts separate.

9. you lap-glue 3 fingerjointed parts together to get your o.a.l. length part which is a long rectangle 6"x12' long.

What am I missing?

One more thing: The way I handle positioning derived parts in derived parts that don't line-up is use the Move Bodies command. But it all depends on your work-flow. I use Parameters to do the move and rotate. Anyways, let me do a quick mock-up to show you how I do it. Maybe this is what you're after?

[cadman777]

The way I handle situations where all the joints have to match-up but they occur on different parts is this:

1. Make one large sheet that's as wide as any sheet will be, and start all sheets from the same side to reference the same finger joint start edge. Then use that as your Template which you derive into all your parts.

2. Derive these templates into a new part, then cut your parts to width and length as needed and add other features.

3. You can make 2 Template parts, one for the ends and one for the middle. So every part references the same edge but they all have a different width, length and shape.

4. The only caveat to this is if you do 'skeletal modeling' like I do most of the time. I do that so all the parts get Grounded in the assembly and few parts need constraints. It helps performance on large assemblies. All the parts fall into position where they're supposed to go, so there's no questions about fits at the end of the project.

5. But if you're doing separate pieces that get constrained in the assembly, there's no need for 'skeletal modeling', and the above method could work for you. If I can see some pics of more of your parts, maybe I can offer a better work-flow.

[Zweerink]

I'm designing the ribs of a complex three-lobed wooden skate bowl, so none of the parts will be square, and most will probably have difficult-to-describe shapes.  Here's a picture of the outside of a bowl similar to what I'm designing:

My (not completely fleshed out) plan is to place the ribs as large pieces and cut away the "blob" that will be the interior of the bowl, and cut again 6" away from the blob so that I only design the blob and end up with the shapes of all my ribs.  I won't sketch and extrude each rib individually.  That's why plopping a split part surface on each rib is so appealing.  I won't even know the rib dimensions.  

More pics:  https://www.dezeen.com/2020/02/18/supreme-store-san-francisco-brinkworth/

[cadman777]

Very nice!

Huge project!

OK, let me get back to you tomorrow b/c my brain's done for the day.

I think my suggestion to make Templates and cut them away is the best work-flow.

That way you can make one and cut to length.

Are you going to individually place them up against the 'blob' and manually trace the cut, then refit and mark the outer edges points and finish straight-cut? Or do you have the 'blog' already modeled and you just need to install all the ribs and use the 'blob' to cope them?

[Zweerink]

I think I may have figured it out.  I made a test part as thick as my plywood, and made a plane between two planes through the whole thing.  Then I split the part so that my 1/2" thick plywood is now two 1/4" thick pieces.  Then I drew a (crude, unconstrained, jagged) sketch of my two finger joints. I will use an iFeature of perfect finger joints for this later.  Then I split the front 1/4" thick piece with the left sketch line, and the back 1/4" thick piece with my right sketch line, then combined the front and back left pieces and combined the front and back right pieces.  Easy!  Then I used Make Part to turn the solid bodies into parts.  

[cadman777]

Excellent! Same thinking as me.

See attached another way to do it using MBP's.

I never use these, but in your case, it seems fitting.

The key to doing all this for me has always been consolidating everything into as small a package as possible and being able to reuse it as often as possible. I like to keep things simple for the fabricators (as well as for me!).

Incidentally, this is one of the things I like about Inventor more than SW. Inventor has a few commands but many applications. SW has many commands but it's difficult to know which NUANCE of command to use in which situation. For me, SW was CONFUSING to use b/c of the myriad of unconsolidated commands. Inventor, on the other hand, can do a LOT with a LITTLE, which is what I like about it b/c I can spend most of my mental energy on designing and detailing instead of making a career out of using my software.

[cadman777]

Here's another version of it w/the 'blob' cutting the part.

Not sure how you handled this.

Your workflow can make or break your assembly performance...