topic Re: How to create body with multiple sketches (cross section and outline) in Fusion Design, Validate & Document Forum

How to create body with multiple sketches (cross section and outline)

Anonymous — Thu, 31 Oct 2019 03:02:05 GMT

All, fairly new user (3 months). Ultimate goal is to model glasses frame for spare reading lenses I have. I have imported the outline.svg and cross section profile .svg into F360 (see attachments). Struggling with the approach to create a body that has the desired outline and cross section curvature.

I thought being clever to just extrude the cross section as a thin body with the desired curvature then it would be a simple matter to Project/Include- Project to Surface and cut the outline profile onto the thin body, resulting in a new body with desired outline and curvature in 3rd dimension. What I've learned is Project does not appear to work if the cutting sketch profile defined plane is not co-planar with the target body defined sketch plane (hope that made sense). In the GUI every time I edit the sketch profile (outline) to Project to Surface the extruded body (based on outline profile) disappears and is not available to target select.

I've reviewed videos/tutorials and also explored 3D sketches, Forms, and Sheet Metal, etc. Unsure what is the strategy to model this deceptively simple object. Thoughts appreciated.

Re: How to create body with multiple sketches (cross section and outline)

davebYYPCU — Thu, 31 Oct 2019 03:25:10 GMT

Two sketches, at 90 to each other, (2 origin planes).

Surface > Extrude the lens curve to cover the lens profile.

Solid > Extrude > Intersect, the profile through the surface.

Read the timeline, with Edit Feature.

Might help....

Re: How to create body with multiple sketches (cross section and outline)

Anonymous — Thu, 31 Oct 2019 03:59:05 GMT

That worked perfectly! Basically extruding with the intersect option. Had the right idea but forgot Extrude has several options.

For my education and perhaps others who read this, is my understanding correct... Project to Surface requires the sketch defining the profile you want to Project, must be parallel to the sketch of the target Body or Surface?

Again thanks very much...have been struggling with this for several nights.

Re: How to create body with multiple sketches (cross section and outline)

davebYYPCU — Thu, 31 Oct 2019 05:38:06 GMT

Project to Surface requires the sketch defining the profile you want to Project,

must be parallel to the sketch of the target Body or Surface?

In general terms that's what happens, but is not a must However the articles being projected must land on the required surface.

The trick of it all is, 2 sketches, the source articles in one sketch. So while you are sending articles to the surface of a body, they are to be contained in their own sketch. You need to create and edit the target sketch and Project (copy deform) the selected articles into it.

Important and is the part not well understood.

Might help.....

Re: How to create body with multiple sketches (cross section and outline)

Anonymous — Fri, 01 Nov 2019 21:54:50 GMT

Sorry to be slow but you lost me on the 2nd paragraph.

"The trick of it all is, 2 sketches, the source articles in one sketch."

Yup, the profile or whatever I'm trying to Project or cut with or whatever in one sketch....

"So while you are sending articles to the surface of a body, they are to be contained in their own sketch."

I think you mean the source entities cannot be in the same sketch as the sketch which defines the target Body.

"You need to create and edit the target sketch and Project (copy deform) the selected articles into it."

I don't understand this statement.

Re: How to create body with multiple sketches (cross section and outline)

davebYYPCU — Fri, 01 Nov 2019 22:33:09 GMT

Sketch 1 has the profile, we are both ok with that.

you want to Project the profile to a surface. How?

Create a new sketch, (this where some get lost)

whilst constructing articles in this sketch (2)

Sketch > Project > Project To Surface,

selecting the profile of sketch 1, is copy deformed onto the surface.

These articles are new articles in Sketch 2.

To Test this, Finish sketch 2, then hide the body, the articles in Sketch 2, do not belong to the body.

sketches to create the body are not involved.

Might help....