Drawing a "gem" - sketch on more than one plane?

tom_auger

I've been following a lot of tutorials and my CAD skills are growing every day. But just when I think I'm ready to tackle a real project, I once again hit against the "this ain't Maya" wall. Clearly, I"m not thinking correctly about these things. Please help.

My current challenge is to model what I'll call that classic "table cut" diamond, with 6 faces, in many ways similar to this image: https://ii.worldmarket.com/fcgi-bin/iipsrv.fcgi?FIF=/images/worldmarket/source/50874_XXX_v1.tif&wid=650&cvt=jpeg (but with solid faces).

My natural inclination is to start on the Top plane, draw a hexagon, then switch to a front plane and connect two neighbouring points and then extend them down on the y axis to line up to the x and z coordinates of the hexagon's center point.

But a sketch can only be on one plane! And if I try to create a second sketch for the next face, the points on the first sketch's hexagon don't "wake up" so I can't snap / constrain to them.

I feel like understanding the "CAD" way of designing this will go a long way to helping me get past my "3D modeler's paradigm" from working with traditional 3D animation software.

Jake_Rosenfeld

Hi @tom_auger ,

You can always "wake up" geometry that is external to a sketch by projecting it or intersecting it with the sketch plane using the "Use" and "Intersection" sketch commands respectively:
https://cad.onshape.com/help/Content/sketch-tools-use.htm
https://cad.onshape.com/help/Content/sketch-tools-intersection.htm

That being said, I wouldn't try to sketch the external structure of this thing if you just want the whole thing as a solid.  I would approach it more prismatically, and just draw three cross sections and loft between them:
https://cad.onshape.com/documents/f701e9fc31a32ded3faf5ba7/w/b3e6a3d7f2561ecf20675d6a/e/6eb860941addd3c21f7910cc


Is this what you meant by "but with solid faces", or did you want something more like a wirefrime/pipes?

Jake_Rosenfeld

@tom_auger

In my original example, the top sketch was a point; Loft will allow you to loft a sketch to a singularity, but it could easily also be done as another small hexagon if that's what you want.



Take a look at this!


I used a bunch of Shell, Plane, and Split features to shell out your part and miter between the faces.  You may have had a different idea in mind of how your pieces are going to fit together, but I think this is a good start.

As always, if you "copy workspace" on my document, you will be able to edit the features to see what their inputs and outputs are:
https://cad.onshape.com/documents/f701e9fc31a32ded3faf5ba7/w/b3e6a3d7f2561ecf20675d6a/e/f2830e5685591d9cf06caa46

Hopefully this is a good guide for your project.  I wouldn't really recommend sketching on 12 planes if you don't need to. 

Jake_Rosenfeld

Hi @tom_auger ,

You can always "wake up" geometry that is external to a sketch by projecting it or intersecting it with the sketch plane using the "Use" and "Intersection" sketch commands respectively:
https://cad.onshape.com/help/Content/sketch-tools-use.htm
https://cad.onshape.com/help/Content/sketch-tools-intersection.htm

That being said, I wouldn't try to sketch the external structure of this thing if you just want the whole thing as a solid.  I would approach it more prismatically, and just draw three cross sections and loft between them:
https://cad.onshape.com/documents/f701e9fc31a32ded3faf5ba7/w/b3e6a3d7f2561ecf20675d6a/e/6eb860941addd3c21f7910cc


Is this what you meant by "but with solid faces", or did you want something more like a wirefrime/pipes?

tom_auger

This is a really simple, but to-scale version of the shape in question, built in two minutes in TinkerCAD (using the "pyramid" primitive).

How could you build this volume in OnShape using sketches and drawing planes?

Jake_Rosenfeld

Hi @tom_auger ,

Did you see my answer above? You can create geometry like this with 3 hexagon sketches and 2 lofts.

tom_auger

Jake_Rosenfeld said:

Hi @tom_auger ,

Did you see my answer above? You can create geometry like this with 3 hexagon sketches and 2 lofts.

Hi Jake, thanks so much for the great info, and also for taking the time to do a quick demonstration sketch - this is extremely helpful to a beginner like me.

I have one question about your technique, and then one concern about that approach. The question is: is that top sketch a single point, or is it a very small hexagon? If the latter, could that be an issue from a precision perspective?

And to my concern: one of my intentions on modeling this form is to be able to derive measurements and angles for fabrication (out of wood or acrylic) - this will also need to include the mitre angles between adjacent faces.

By modeling this as a solid, I'm not sure I will be able to take those measurements, and the faces themselves are 1-sided. I realize that in my original post, I talked about a "solid volume" and that was actually a mistake to describe the final geometry in those terms. Essentially, I need to be able to model each facet as a solid (extruded trapezoid).

I will try the "use" approach, but it will be a challenge working on so many different planes and having so many different sketches. Am I missing another basic tool or approach in the OnShape toolkit?

Thanks,

michał_1

One sketch and two extrudes:
https://cad.onshape.com/documents/7b6fdcc4f0c0c0f4fce1e347/w/950d6e0b561e8ff1345324d2/e/d799f8edde954268b394e4f9

Jake_Rosenfeld

@tom_auger

In my original example, the top sketch was a point; Loft will allow you to loft a sketch to a singularity, but it could easily also be done as another small hexagon if that's what you want.



Take a look at this!


I used a bunch of Shell, Plane, and Split features to shell out your part and miter between the faces.  You may have had a different idea in mind of how your pieces are going to fit together, but I think this is a good start.

As always, if you "copy workspace" on my document, you will be able to edit the features to see what their inputs and outputs are:
https://cad.onshape.com/documents/f701e9fc31a32ded3faf5ba7/w/b3e6a3d7f2561ecf20675d6a/e/f2830e5685591d9cf06caa46

Hopefully this is a good guide for your project.  I wouldn't really recommend sketching on 12 planes if you don't need to. 

tom_auger

Jake - again, extremely helpful. You have my gratitude for taking the time!

I've got a copy of your project open here and I've set up a new part studio to try to replicate your workflow in every detail to gain a full understanding of it. So far so good.

I'm wondering though how I'm going to go about getting those 50% miters. In your example, you have what appear to be butt joins (eg: the bottom), and I'm curious if there's a way to control how those pieces join up. It may become obvious when I dissect your project further, but if you have any advice on the matter and the time to compose an answer, it would be greatly appreciated. Edit: I see that one could use splits again with custom planes to create whatever miter angle you want, but that seems really tedious for more complex projects. Here we seem to have to create only 6 additional custom planes in order to get those 6 bottom miters, but I'm wondering whether there isn't a more automated way to do this?

Thanks again!

Jake_Rosenfeld

@tom_auger

For something with circular symmetry like this you could set up one splitting plane and then do a circular pattern (feature pattern of the plane feature).  That may be easier than setting up all 6 planes directly.

Stuff like this is also sometimes easier to program mathematically in FeatureScript, rather than going through the UI, but I'm not sure if that's something you'd be interested in?

Jake_Rosenfeld

With the circular pattern mentioned above in mind, it could just be easier to design one "slice" of the diamond and then circular pattern at the very end:

https://cad.onshape.com/documents/f701e9fc31a32ded3faf5ba7/w/b3e6a3d7f2561ecf20675d6a/e/8cae93c8565e47b30ae83eff

tom_auger

Jake_Rosenfeld said:

@tom_auger

Stuff like this is also sometimes easier to program mathematically in FeatureScript, rather than going through the UI, but I'm not sure if that's something you'd be interested in?

I'm actually a coder, so this is definitely something I will be interested in exploring once I have the modeling basics down!

Thanks so much for the advice and the many options you have presented.