Transform, can't select anything? Convert to solid?

apearce

When I select the transform tool I can't select anything:
https://youtu.be/g6H4O7XmYzE

I hope this isn't a rookie mistake. The sketch was imported from an DXF if that's related? It seems the object is not a true parasolid? A bit like a mesh but it's not a mesh... 

I want to move a point in order to make the wing narrower at the tip and wider at the base. 
AFAIK I need to convert to a true solid. 

jakeramsley

From watching your video, I believe the wing is defined off of Sketch 1.  You are creating new sketches and then trying to transform the face or edges of the solid model, and not entities in the sketch.  Double click on 'Sketch 1', which should put you in edit mode for Sketch 1 and from there you can deform your sketch to change the shape.

Jake_Rosenfeld

Hi @apearce ,

If you share the URL to your document here it'll be easier to help with your request.  Looking at your video, the issue isn't that you don't have a true solid. Your solid is fine, the source of the sketch won't affect the validity of the part itself.

The issue here is that sketches are only used for creating new sketch geometry.  By picking the top plane of your part, you will only be able to sketch new entities on that plane for later use, you would not be able to move any of the geometry of an existing solid.

I think the best option for you here would be to approach making this part in a different manner: you could import your original sketch,
place it on the 'top' plane as you've already done, then use the 'offset plane' option of the 'Plane' feature to create another plane above the top plane, and create a sketch that looks like what you want the other end of your fin to look like (The sketch 'Use' command will be helpful).  Then loft between the two profiles to create your final part.  If you use this method, you will be defining exactly the profiles you want for the two ends of your fin, and there is no guesswork or inexactness of just moving vertices around.  Here are relevant help docs and an example:
https://cad.onshape.com/help/Content/cplane.htm
https://cad.onshape.com/help/Content/sketch-tools-use.htm
https://cad.onshape.com/help/Content/loft.htm
https://cad.onshape.com/documents/56964a64d214d745a06f24ad/w/ebb693d1cdb71e773412f2f0/e/e1490bbc706a579294f7dd43

Another simple option that may give the geometry you want (I'm not sure exactly what your desired outcome is) would be to use the 'Draft' feature with the bottom plane of your fin as the 'Neutral plane' and the side faces as 'entities' so that you can create an angled draft of all those side faces:
https://cad.onshape.com/help/Content/draft.htm
https://cad.onshape.com/documents/56964a64d214d745a06f24ad/w/ebb693d1cdb71e773412f2f0/e/05b11d0d122bd5261059871b

A last option may be to use the 'Move face' feature to rotate the face you want to change, but I think this is a little too complicated for what you need, and the two options above are probably better anyway.
https://cad.onshape.com/help/Content/moveface.htm

As always, if you copy the document I've shared here with examples, you will be able to edit the features so you can see what inputs I used into them.

apearce

Thanks for the reply. Been a bit delayed. Don't really want to ask for help again also really but I can't get my head around it still and I don't know what else to do. 

Offset plane method: I select the face of sketch 1, plane, offset, click the tick but then no duplicate is seen in the object list. Just doesn’t appear. I don’t know how to give any more drag info. 

“plane 1 did not generate properly. too many entities were selected” happened at first but then I tried with just the face of the sketch selected. Now I have a plane but nothing on it from the sketch imported. 

Here’s the doc:

 https://cad.onshape.com/documents/37c184ca6da6b9a800e89144/w/45f5790ff82ea4a37fbd283e/e/3416bcce4556e5ecfea329a0

You'll notice that the imported DXF I drew with Inkscape using only 3 vectors has a lot of vectors. I guess that's an inkscape problem though rather than the import process. Probably a complication of DXF versions (SVG import would probably be simpler is my guess)

Sorry for such idiots questions. 

Jake_Rosenfeld

Hi @apearce ,

Now worries about the follow-up question.  I think my answer was a little dense anyway.

"offset plane" will not imprint any of the sketch geometry from your sketch.  It will just create a new plane that if offset from your selection.

My advice for you is to:
1) Place your imported sketch on the "Top" plane (as you've already accomplished)
2) Make an offset plane off of your "Top" plane
3) Start a new sketch on the newly created plane
4) "use" the edges of the original sketch to imprint them onto your new sketch plane
https://cad.onshape.com/help/Content/sketch-tools-use.htm
(now you'll have the imprint you want)
5) click "show constraints" in the sketch dialog
6) For the points you want to deform, click on their constraint, then press backspace/delete (windows/mac).  The constraint will look like this:

you may also have to delete the constraints on the 2 edges around the point you want to deform
7) The point and its surrounding edges should now be blue.  move them around as desired to design your end profile
8) Loft between the two profiles
https://cad.onshape.com/help/Content/loft.htm



If you were just looking for a simple angled taper rather than selectively moving a couple points around, there are simpler ways to do this, such as just using extrude with the "draft" option