Create sketch from extruded body face not producing an editable sketch

[MrX2111]

Hello,

I see videos of people creating sketches from a body face without issue. If I create  a cube, select a side, right click create sketch the sketch it creates looks to be just a profile and not editable even though I can select the edges and points when hovering over them or right clicking.

What am I doing wrong?

[g-andresen]

Hi,

To use a profile in a sketch, it must first be projected into the current sketch (e.g. with the key combination P).

Please share the file for investigation.

File > export > save as f3d on local drive  > attach it to the next post.

günther

[MrX2111]

here ya go

[g-andresen]

Hi,

project body profile into sketch 2

günther

[MrX2111]

I used a simple cube just to demonstrate what I was trying to do but in reality I am working with a more complex shape that I was hoping to avoid having to retrace to continue working from a specific face. Am I just not understanding clearing what create sketch from face is to do? Is it to result in an empty sketch planar to the face or is it supposed to bring the geometry over as well as a starting point?

[Bunga777]

To edit a profile sketch, right-click on the sketch in the browser and select "Edit Sketch.

The same operation can be used to edit the sketch in the history below.

[laughingcreek]

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@MrX2111 wrote:

... sketch it creates looks to be just a profile and not editable even though I can select the edges and points when hovering over them or right clicking...

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That is happening because you have this (by default) in your preferances-

which projects the edges of the body as sketch elements into the sketch, but AD chose to make those projected elements invisible to, quote "reduce clutter".  I've lost track of how many people this has tripped up over the years.  and if you ever create a sketch on a face that has a bunch of edges you can even crash the program, or at least make it laggy. 

I HIGHLY suggest turning this preference off,  and discreetly projecting into the sketch what you need to use as @g-andresen describes. 

[Bunga777]

I think the reason I make sketches on the Surface is simply because it is easier to understand.

As long as it is consistent with the direction you want to push out, you can draw your sketch anywhere on the XZ plane or on the Surface.

It is best to draw the sketch in a place that is easy for you to understand.

You can also do exprude without starting from the plane you have sketched.

Video.

https://knowledge.autodesk.com/community/screencast/89024504-2d4c-45fd-aaeb-4dc4d9d7bf0d

[MrX2111]

Let me use a real use case which I am working on. The attached file will have an object that looks like 2 ribs. How would you cap the top like the photoshop file I attached "ribs capped". "ribsA" is the before.

PS: I checked the setting and auto project geometry is not checked.

[laughingcreek]

when ever possible, you want to refer back to originating geometry, in this case the sketch.  see attached model.

There is also some weirdness going on with that first sketch, you have curves laying on top of each other in both ribs-

Also, curvature quality will suffer when you use sketch offset on a spline.  I suppose not a problem here, but will be when are doing surfacing work with lofts-

[MrX2111]

What is the best practice in lieu of offsetting splines?

[laughingcreek · Accepted solution]

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@MrX2111 wrote:

What is the best practice in lieu of offsetting splines?

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There are a variety of options depending on what the need is.  if you don't need the line or an edge created from the line for something else, then doing it with the sketch may be good enough.  but if you need to use it for a sweep, loft, etc . later the reduced curvature quality becomes problematic.

the work arounds involve using solid/surfacing command features instead.  such as: creating a surface and offsetting the surface, using thicken or shell, using thin extrude. and probably others.  the one you use will depend on the circumstance.  in the attached I used thin extrude. (the 2nd extrude in timeline named "extrude 3")

[davebYYPCU]

Seems this thread went off topic, 

You selected the top of one body to make the second sketch.  That body is / was projected to the sketch, only blue profile is visible when you hide the body.  (I also broke the original profile with a line changed to construction)

To successfully place a cap over the 2 bodies, you project the outer curve of the other body, and close the profile for the top plate.  Extrude this to height required.  I joined it to both ribs in the Extrude process.

Added black and purple lines to your sketch.

Might help....

[MrX2111]

So I think this gets to the heart of it. After you project the outer curve of the 2nd body did you have to retrace it or was the geometry there for you to join it by the ends?

[Bunga777 · Accepted solution]

Double-click on Sketch2 to enter Edit.

In the edit window, use the projection to copy each surface.

The contour of each body is projected in this way. 

Connect the ends of the projected lines with new lines to block the area.

All that remains is to Extrude.

We took a video of the work, click here to see the video.

https://knowledge.autodesk.com/community/screencast/e9448794-06d6-413b-a990-f65380dfa77f

[davebYYPCU · Accepted solution]

The purple lines in the sketch are the result of Project > Project.  Linked to the outer curve of sketch 1, so edit sketch 1 will update the purple lines.  The black lines connected automatically to the original shaded blue boundary corner points, (end point of invisible lines, mouse highlight them to see them) and the purple end point/s.

Bunga says project the second body but that brings in more purple sketch articles that you didn't need, to make a top plate.

Might help....

[MrX2111]

First off thank you all for taking the time with the noob, you guys are great! Never had a forum so helpful so quickly. The point I was missing was that the projection itself could be used. I thought when a profile was projected that it was meant to be  projected on to the new sketch just as a template to be traced (which is why one of you found double lines).  When I click create sketch and clicked on a face it just gave me a profile tinted blue and I did not see any lines. In the videos I have watched it always seemed like they had actual lines to work with after the projection was created.

Again thanks!

[Bunga777]

hi, @davebYYPCU 

You are certainly right.

It is certainly better not to add more sketches that are not needed.

On that note, good point about that projection being unnecessary.

[davebYYPCU]

It is subtle - create reference projection on sketch create as per Preference, 

Fusion does not draw visible lines, so unless you go looking for them, you won’t see them until you mouse over them..

however if you manually use the Project tools, you get purple articles.

Your videos are either very old, when the purple lines were provided both / either way, or you are seeing manual projections, and not the ones making invisible lines.

Takes a while to explain, new people (and those of us who saw both options) find it intuitive - Not.

[laughingcreek]

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@MrX2111 wrote:

...When I click create sketch and clicked on a face it just gave me a profile tinted blue and I did not see any lines. ...

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you should check again if there is a check mark next to "auto project geometry on active sketch plane" in your preferences.   This setting being checked at the time a sketch is created is the only way I know of to create profiles with invisible lines in fusion.