Questions about tangent arc, extrusion and explanatory text

mark_nahabedian

I have some more questions about OnShape.

Here is a link to my document:

https://cad.onshape.com/documents/87c734434a3d09a1007f9322/w/822165c65a73fcefc6d8feb9/e/8f26de91098948b7dd2b8275

1) In the "elevation" sketch of the "stop nut" part studio I have an

elongated "S" curve to define the profile of the part.  I used a

short line and two tangent arcs to draw this profile.  I tried

just drawing it with two tangent arcs and no middle line segment

but couldn't get the two arcs to be tangent to each other at

their meeting point.  Is there a better way to sketch this "S"

profile?

2) As shown in the "plan" sketch of "stop nut", I want the nut to

have a pentagonal head (the nut will be threaded 20 per inch, so

each corner of the pentagon advances the nut by 0.01).  Ive not

yet found a way, using the extrusion tool in the sketch, to cut

the 5 sides of the head away from the result of the "revolve"

tool.

Using the "solid" tab of the extrude tool, I'm unable to select

the regions that are bounded by the outside arc and an edge of

the pentagon.

If I try the "surface" tab I can select the circle and the

pentagon edges and extrude that, but that gets me a hollow walled

extrucion and no option to remove that region from the part.

If I were instead to shorten the revolve and extrude the pentagon

on top of it, then the corners of the pentagon wont carry the

curve of the profile.

I tried extruding in the part studio itself, rather than in the

plan sketch.  That didn't work either.  See "failed Extrude 1".

I doesn't look like I could achieve what I want using the boolean

intersection tool unless I define the pentagonal head as a

separate part.

What Is the best way to get a pentagonal head on my part?

3) Also, is there a wat to add instructional or documentation text

to a sketch or part?  I dont want the text to appear on the part

itself, just in the drawing.  Example text might be "Tap to 1/4 -

20".

Thanks for your help.

steve_shubin

@mark_nahabedian

https://cad.onshape.com/documents/9cea1e5387469ba4690f61a0/w/53dd1081a882efd2e75ebeb7/e/c3c85fc47b403011bff2fdb4

I think this is what you were trying to do. But I could be wrong

But after extruding to make the five sided nut, it takes away most of that tangent S shape. So ... ?

The two arcs both have radii that are vertical, parallel, with points that are coincident, hence they are tangent.

As far as your question three, I’m sure you could add text in a drawing. Or you could write a document and save it as a PDF and import it and that PDF will have its own tab

steve_shubin

@mark_nahabedian

The two arcs made tangent faces

mark_nahabedian

Thanks Steve.

I want the comment text to appear on the sketch where it is relevant, not in another page one will never look at.

I cant begin to tell you how much I despise PDF files.  People hardly ever read documents on paper anymore so PDF is obsolete.  Try reading one from your phone some time.

I don't understand what you did to get the result you got.  I want to understand why extrude, solid, intersect, through all of the pentagon doesn't work for me ("failed extrude 1").

tim_hess427

@mark_nahabedian: You'll need to make a couple of changes - 

1. Change the "body" revolve to "Solid" instead of "Surface". You'll need a solid part in order for the intersect to work correctly in step #2. 
2. For the extrude, you'll want to only select the pentagon face from your "plan" sketch. Right now you have both the "plan" and "elevation" selected. Then flip the extrude direction and select "Part1" for the Merge Scope. 
   

There is a tool to add text to a sketch, but it is not really intended for annotations (more for things like engraving). General functionality for adding annotations directly to 3D models is something that has been discussed (debated) and requested, but the functionality does not exist currently in Onshape. 

bruce_williams

@mark_nahabedian

1) On your 'S' sketch you should define constraints so it is all black.  As to making two arcs tangent, that is easily done.  I think you have an extra horizontal constraint (see pic below for tangent arcs and highlighted horiz constraint).  Just delete that constraint and dimension the arcs as needed.


2)  Your Revolve should be made as a Solid.  Then the Extrude 1 can be set up as intersection as I have on this document.

3) If you do not want to make a drawing with notes - you can add text to a sketch (same or other) OR use the Comment feature (see my document with with sketch text and comment tagged to the elevation sketch).

bruce_williams

@tim_hess427 I see we posted at same time - great minds think alike!