Sculpting a Vambrace

[Zero__]

Hi guys -

I'm creating a wearable piece of technology that fits along my forearm, like a simple vambrace. And I have to create indentations in it to embed some microcomputers and PCBs. A friend at Autodesk suggested I try to use the Sculpt to instead of my usual hack and slash boolean CAD modeling. It's going slowly but well..I'm kind of getting the idea of pushing and pulling faces to rough out the shape I want, then cleaning it up in the traditional modeling environment.

I'm struggling with one thing though. I create a conic and then push in the faces to create my indentations. But the bottom of those indentations needs to be flat, and it is of course conic now. Is there a simple way within the Sculpt environment to make my pushed-in-indentations have flat (planar, parallel to my bisecting plane) bottoms?

Thanks!

[Anonymous]

@Zero__

Hello maybe you can try this workflow. At the Create Form Mode you might not be able to get the indentations you wanted. But you can extrude at the Parametric Mode to get the correct shapes.

First you should construct, offset and move  planes at the Create Form Mode to the correct positions (you should move the construction planes at the Create Form Mode. This is the only way you can move the planes to any postion you wanted). Taking notes on the distance from the surface. I would suggest you to Thicken your model to the correct thicknes before you did all these. Then you project the edges or entities you wanted to the created planes. You can then "Finish Create Form" and go back to the Parametric Mode.

You can Extrude into your model from the planes and select the cut option. This is only one of the ways. There are others. A few screen shots here:

1. Construct, offset and move planes to the correct positions. Project the entities you wanted to the planes.

2 Finish Create Form and then Extrude into the body with the Cut Option:

3. This is the result:

[TrippyLighting]

I am not at my Fusion machine at the moment but I am pretty sure there is a "Flatten" command somewhere.

[TrippyLighting]

Yup.

Here it is 😉

[Zero__]

Thanks a lot guys. @Anonymous, I used a modified version of your workflow, that was helpful. I did end up switching back mostly into the modeling environment - coudn't quite figure out how to do what I needed to with the Sculpt environment.

I have another question related to this vambrace. I went ahead and lofted together two circles to make the general shape, then I used tangent planes and sketching to create some flat pads on the side. Now I need to make a wall around those flat pads. The workflow I'd use in my old CAD package was to:

• Thicken the conic Surface but create a New Body out of that thicken.
• Use planes angled around the axis of the cone to Trim it to size.
• Finish it off with a Shell command. Unite my body into this one and boom, walls around my pads.

This isn't working in Fusion. I tried to use the Thicken tool but it apparently won't work on the face of a solid body. I tried to use the Offset tool but the option to create a New Body wasn't there. So I thought ok, I'll just make a new Surface overlaid on the surface of my conic. Not a very clean method, but it would do. I couldn't Extract the Face to make a new surface, nor could I Revolve a curve to make a surface!

I'm struggling to translate my old workflow into Fusion. Any idea what process I should take?

EDIT: Ok, so I gave up and created that New Body by lofting larger circles together. Then I planned to cut it to size using Planes. I'm so used to the Trim tool in NX. Only to find that no tool seems to exist that's similar? Is there a way to Trim or Cut a body using Construction Planes in Fusion 360?

[Anonymous]

@Zero__

Hi, good to hear that our suggestions worked for you. I believe the good thing about Fusion 360 is that it can switch between all those modes.  "Thicken" only works in "Create Form (Sculpt)" and "Patch Mode". It does not work on a solid body. But you can "Convert" a solid face into a T-Spline and then you can edit in "Create Form -Sculpt" mode. You can then thicken the T-Spline and when you "Finish Create Form" it will change into a solid. Sometimes you can use "Replace Face" command to replace a Solid Surface by the Converted T-Spline Surface that you had edited. Besure to make the T-Spline Surface bigger then the Original Solid Face to be replaced. A few screen shots here to demonstrate the using of "Convert" and  "Thicken" commands. Then Changed back to Solid again. I changed color in between for easier viewing:

1) For example a box is created in the parametric (Modeling ) mode:

2) I selected "Create Form", the solid body changed into something like a Translucent body, I selected a face and used the "Convert" Command to convert it:

3) A converted face :

4) Thicken Command was used here:

5) After "Finish Create Form" a New Solid Body is formed. You can Push Pull or do anything on this new body. It is not combined with the original one:

[Anonymous]

Hi I believe "Offset" works on sketches only. I do not think it works on solid bodies at this time. Maybe in some future updates.

[Zero__]

I find that Press/Pull became Offset Faces when I selected the conic face; unfortunately it did not have an option to create a new body out of the Offset. That much is usually reserved for the Thicken Command. Just strange that the Thicken command would not work on the face of my solid body.

[Anonymous]

@Zero__

Hello to offset a new body from a conic face, I can suggest two methods, there are few other ways to do thatas well. First suggestion is to convert the conic face into a T Spline, thicken it and then change back. You will ended up having two separate bodies.  For example, I used a Solid Cylinder to demonstrate.  Using this same Cylinder the second suggestion is to project the flat side of this cylinder to a plane. A circle will be projected. You then select to Offset this circular sketch, then you can extrude that into a new body or component. The Convert example is shown in a few screen shots

1) A solid cylinder is formed. The face of the Cylinder is converted into a T Spline:

2) While still in Create Form, Thicken was performed. After "Finsih Form" two separate bodies are formed. I moved them out to demonstrate:

By the way the good thing about Converting to a T-Spline is that you can sculpt the T Spline by Edit Form command. Then change back to Solid.

The other suggestion, the Project-offset curve-extrude workflow can make a solid body also. But if you want to Sculpt it you will have to convert the face to do that. 

[Zero__]

Thank you! That's enlightening. I tried to use Convert before in my efforts to generate a face from my body, but it wasn't working. I could not figure it out till I paid close attention to your screenshot and saw that you had to select Brep bodies. I ended up using the rather messy method of creating additional Lofts and then "trimming" then down using the Combine tool. I may remodel it this way, it would probably make my workflow much cleaner.

[Anonymous]

@Zero__

Hi I hope you enjoy using Fusion 360. I had been using this program to design beautiful things for ladies. Including limited edition Perfume/lotion bottles for European Skin Care Product Companies. This program can make beautiful things easier because I could concentrate on designing and less on engineering.