topic Re: I am stuck with a CAD design, bend a model or sketch into curved body. in Fusion Design, Validate & Document Forum

I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Wed, 09 Oct 2019 15:11:54 GMT

I need to “bend” a 3D model or sketch onto a curved body. I don’t believe there is a way to directly do this in Fusion, but I am wondering if any of you “gurus” can think of a work around or a way to fake it this time.

Here is the situation - We are a snowski manufacturer. All our engineering, design, and manufacturing is done here in house. Although we are producing a 3 dimensional product, our CAD is mostly 2D.

We do some 3D CAD which we then machine on a 3 axis router. Other than that, most of our tooling is created using 2 and 2.5 axis strategy. On the engineering end we have never drafted a 3D model of a pressed ski.

Right now I am in a situation where I need to machine a ski after it is taken out of the press. This means that I will have to model a 3D, pressed ski. From that I will design some hold fixtures and finally create 3D milling operations. My biggest holdup right now is determining how to create this 3D geometry.

To give an idea of our build process, we prepare all the components in a flat plane - ie the plastic base, wood core, composites, etc… These are all put into a press with epoxy. Once the epoxy cures, the components are molded together in the shape of the mold.

My hope is that I can use the existing CAD geometry for our mold and our flat shape to make either a 3D model (preferred), or a 3D sketch on the mold (also will be greatly helpful). To better illustrate my situation I will provide examples that I do have CAD data for and an example of a pressed ski, to which I am trying to model in Fusion.

Ski press - this is where the flat components are pressed with an epoxy and come out with the press profile.

CAD for the ski press, what I hope to use to “bend” the sketch or 3D model.

CAD for the ski shape, what I hope to “bend” into the mold.

Pressed SkiPressed Ski

Here are some pressed skis, this is what I am trying to create in CAD.

I hope this makes sense. I know there is no direct way to do this in Fusion but I am open to just about any idea or method someone has to make this happen.

Thank you!

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

wmhazzard — Wed, 09 Oct 2019 17:54:23 GMT

What you need to do is draw the side profile of the bent ski and extrude to the width. Here is a picture and a file of an example.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Wed, 09 Oct 2019 18:09:53 GMT

To get the thickness, camber, etc.. of the ski this method will work. However where I am stuck and was stuck when creating this thread is "bending" or "deforming" (sketch 2) in your example to get an accurate tip/tail and sidecut shape.

Since we design the sidecut, tip and tail shape in a flat plane it will not accurately extrude to the bent shape (sketch 1) in your example. It would go off the ends of sketch 1 by a few centimeters.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

TheCADWhisperer — Wed, 09 Oct 2019 18:54:55 GMT

If this were my design I would see multiple dimensions on the sketch.

I would have the Origin Center Point at the midpoint of the bottom Horizontal line.

I would have a Horizontal Constraint on that horizontal line.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Wed, 09 Oct 2019 19:23:16 GMT

All the CAD design is done in AutoCAD and imported into Fusion. The Fusion 360 sketch environment is not quite robust enough to handle the way our designer works. We have tried designing in Fusion and run into sketches that would not solve. Most of this geometry is ellipses not just arcs and this is part of the hangup.

This is why you don't see any constraints in the drawings.

For any 3D work and most of our CAM work Fusion is the go to software and I think the only software in our quiver which is capable of creating a design like we are trying to achieve.

If these drawings were fully constrained do you think that we would be able to "bend" the sketch or model into the "mold"?

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Wed, 09 Oct 2019 19:32:22 GMT

Perhaps to simplify my request -

Is there any way to "bend" or "form" the sketch into the body, the "mold"?

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

davebYYPCU — Thu, 10 Oct 2019 04:19:30 GMT

You have a 3d model of the lower mold,

presume you have a similar upper mold.

If you place both in space, the cavity becomes the third 3d model, of the set.

You can't bend a sketch, but you can obtain the section sketch of the models in place.

Otherwise I would need the file /s to assist further.

Might help....

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

TheCADWhisperer — Thu, 10 Oct 2019 06:39:32 GMT

@Cave_Master wrote:
If these drawings were fully constrained do you think that we would be able to "bend" the sketch or model into the "mold"?

I suspect that I would be able to accurately model with fully constrained sketches.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Thu, 10 Oct 2019 14:47:41 GMT

I do have geometry of the upper mold and could easily extrude a model, however this will not help us. The upper mold is pretty generic. In the OP, do you see the yellow fire hose looking material in between the top and bottom molds? This is an air bladder that takes the place between the ski profile and the top mold. The thickness profile is dictated by a different profile sketch. The molds dictate the "camber" and "rocker" profile.

Also coming up with the side profile showing the thickness and camber/rocker is relatively easy with lots of segmented offsets, compared to the issue is deforming the flat shape into the mold so that I can have an accurate sidecut, and tip and tail shape to work with.

I will reach out to you in private message about files.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Thu, 10 Oct 2019 14:45:44 GMT

Do you think that if I had a fully constrained sketch that you could then "form" the sketch into the curved body?

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

g-andresen — Thu, 10 Oct 2019 15:22:32 GMT

Hi,

maybe this thread can help you with your considerations.

günther

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

TheCADWhisperer — Thu, 10 Oct 2019 15:43:34 GMT

@Cave_Master wrote:
Do you think that if I had a fully constrained sketch that you could then "form" the sketch into the curved body?

I make use of 3D sketch intersections (Project Geometry).

If you are going to model this board and tooling in Fusion 360 - I think that you will have to model in both flat and molded form. Otherwise I think you might need to look at something like Autodesk Inventor Professional.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Thu, 10 Oct 2019 15:40:11 GMT

Interesting. I may be able to use some of these techniques to come up with something close to what I need.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

wmhazzard — Thu, 10 Oct 2019 17:11:13 GMT

Here is one way to get a sketch that conforms to the body that you need. I did a split face with the planer sketch. Then I opened a new sketch and clicked project, include 3d geometry and clicked on the faces of the body where the original sketch was. That gives you a 3d sketch that you can send to your cnc machine. See attached file.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Thu, 10 Oct 2019 18:34:21 GMT

To be geometrically accurate, the ends of the projected sketch would not come to the ends of the flat sketch. The curved sketch if flattened would actually be stretched. Think if you had the physical mold, and the flat sketch printed out 1:1. If you set the print out on the mold it would be slightly shorter than if had the print out laying flat next to the mold. This difference is a few centimeters and accounted for in our design process, is a 185 cm ski might have a flat length of 189 cm.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Thu, 10 Oct 2019 18:44:23 GMT

Do you have any advice to model in "molded" form?

What feature in Inventor Professional could I use to form a body or sketch into a curved body?

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

davebYYPCU — Fri, 11 Oct 2019 00:10:08 GMT

Fusion can do it.

Using your sketches, but not sure of dimensions for some things

Cut edge method?

Also not sure of the way you cut the edges, with this method, or with a vertical router / mill

File Attached, step up the timeline. should get you going....

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

wmhazzard — Fri, 11 Oct 2019 01:42:46 GMT

Now I understand what you want. You can bend the sketch using sheet metal. I made a sketch and projected the side of the mold and used that line for the flange tool in sheet metal which gave me a sheet metal body which can be unfolded. I then used the 2d sketch to cut the sheet metal body to size, then re fold the body. Then you can project the surface on a sketch.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

Cave_Master — Thu, 17 Oct 2019 00:58:28 GMT

@davebYYPCU , @wmhazzard

Those solutions make a lot of sense. Thank you so much for putting the time in to help me figure this out.

I had never really used the sheet metal function, I familiarized myself over the weekend. I have been trying to fit in some design time but have been slammed with work on the floor. I have been able to put in a little work on this here and there. Fortunately I am able to "cut" the flattened mold and refold it. This will give me enough geometry to make the most basic toolpath, so I am happy. However, Ideally I would like to take this to next level and run some boolean operations (intersect) and make an actual 3D representation of the ski (thickness, sidecut, and camber (which this sheet metal trick has shown me). I can't figure out how to run an intersect and then refold the model. I have attached a screencast showing my roadblock.

Re: I am stuck with a CAD design, bend a model or sketch into curved body.

wmhazzard — Thu, 17 Oct 2019 02:17:35 GMT

Instead of trying the join command, make a new body in the shape of the ski and then go to the solid workspace and use the combine tool. Make sure to select the sheet metal body as the target body and the solid body as the tool body, that will make the ski body part of the sheet metal body which then can be re folded.