Text use questions/issues/tricks.

laird_broadfield

1) As you can see here, I'm looking at the back of the right plane -- text one and text two are on the right plane.

I want text two to be on the *Back* of the right plane, so that it appears correctly to the current viewer.  I've tried fixing a corner of the text and dragging another corner to flip it (no); I've tried specifying the sketch plane while viewing from the desired perspective (no), etc.  The only workaround I've found is to create a physical part (not just a plane) that has the surface I want, and then sketch on that, but that has downsides.



2) If I extrude text as a new part, I don't get a new part.

I get 67 new parts.  That actually makes some sense -- but I can't figure out how to subsequently readily treat them as one part.  (Tried boolean union, but they don't touch.)  Even if that worked, subsequently editing the text causes a nightmare of lost and orphaned parts.  Better way?



3) I figured out a way to emboss uniformly on a curved surface, but I'm curious if there's a better way.

Take ugly gray cylinder:


Sketch the lettering on a tanget (or tangent-ish) plane, and extrude to the part surface:


Translate (all 37) letter parts into the surface an appropriate distance:


Subtract (all 37) letter parts from the main part:


This might be obvious to the pros, but I had to figure it out; maybe this helps somebody.  (At least, until there's curved surface sketching.)  You'll get some distortion at the radical extents, but it's manageable.

traveler_hauptman

Regarding (1): As you are discovering, a sketch only works with one side of a plane and Onshape has no way to distinguish between sides. You can create a second plane that is flipped as shown in this example. Warning: The technique I used for flipping the plane (rotate about axis) is not well behaved. Onshape knows about it and will hopefully be fixing it.

(2): Onshape does not yet have a good way to work with lots of parts. (It should!) Until improvements come, careful use of box-select will reduce the tedium.

(3) That's a great illustration of how to do it. I'm sure it will help a lot of people.

shashank_aarya

@laird_broadfield Regarding (1) I also used same workaround method what you have described. You can create just a surface not a part which can be used to create a text on it. After creating a text you can delete it. It will appear in feature tree as "delete part". So, surface created for text will not appear to annoy again throughout the modeling unless and until you delete the feature "delete part"

Regarding (2) I think practically it is not possible to have multiple unattached solid bodies as one part. So, approach of Onshape is perfect.

Regarding (3) I would suggest one workaround as below.

Step-1 Extrude the text into the cylinder at maximum depth


Step-2 Create another cylinder as a new part inside first cylinder in such a way that it intersects all the parts created by text.


Step-3 Make Boolean subtract to remove the second cylinder from text part


Step-4 Again make Boolean subtract to remove text parts from first cylinder to get the text protruded along cylinder curve.

jakeramsley

For #3, I would take advantage of the replace face, move face, or boolean with offset command.  That way you can offset them about the normal of the cylinder, keeping the capped face cylindrical as well.  By doing an extrude up to surface, the terminating faces already have the cylinder underlying.  Offsetting them inward should move them all in towards the center of the cylinder.