Why is this letter not extruding?

tom_seibold

I imported a DXF from Illustrator so I could emboss a logo on my part. It came in perfectly except for the last letter, a capital C. After trying various other settings, I resigned myself to the C's inexplicable non-importability and duplicated the existing paths (sorry, using AI lingo) of one of the Os and moved it over to where the C was supposed to be, and modified it into a C.

The C looks fine in the sketch, but I notice that its outlines do not "highlight" (as the outer part of all the other imported letterforms do) when I mouse over the drawing area. It's like this part of the drawing is not being included, or recognized.



And when I extrude, the C doesn't appear. I can create other new shapes on the drawing and they instantly extrude, but the C will not under any circumstances pop out. Any ideas why?

bruce_williams

The 'C' geometry must not be a closed region (there must be one or more small gaps at the segment end points).  You can narrow down the problem by drawing temporary lines across the C and see what does not shade into a closed region.   Then repair with another segment or a Coincident constraint. 

  

owen_sparks

Hi and welcome. If you post a link to your document (just cut the URL it of your browser and paste it here) then I'm sure someone will take a look for you.

In the mean time is that area of the sketch shown in grey? If not to have a small opening somewhere.
Cheers, Owen.

bruce_williams

The 'C' geometry must not be a closed region (there must be one or more small gaps at the segment end points).  You can narrow down the problem by drawing temporary lines across the C and see what does not shade into a closed region.   Then repair with another segment or a Coincident constraint. 

  

romeograham

@bruce_williams
That's a nice tip (drawing the temporary lines)!

tom_seibold

@bruce_williams and @owen_sparks: I appreciate the tip. I thought I had examined my edited "path" (Illustrator-speak) very closely and fixed all coincident point problems before posing my question on this forum. However (Bruce), your technique of drawing segments helped me locate a "gap in the fence" and fix the problem.

But it's not quite that simple. As shown in my first screenshot in my original question (above), my sketch paths are being drawn on an existing extruded part, and the light-gray shading that helps you troubleshoot open/closed-region issues in the way you described is not visible against the shaded part the sketch is being made on! This is further illustrated by a test rectangle I drew on another plane, which spans both a shaded part and open space (white background) behind. On open space (right), the shading is very easy to see. Against the part (left), it is nearly invisible! 



Suppressing the extruded part that my (logo/lettering) sketch is on doesn't help--Because my lettering is on a sketch drawn on that extruded part's plane, suppressing the extruded part makes the sketch go invisible, too.

So the only way I could figure out how to troubleshoot my open region problem was to move the letter off the part and onto an open space to the side where I could see the light-gray shading as I drew the intersecting lines. Is there a better technique that would allow me to see the shading / troubleshoot sketch regions without temporarily moving the segments off the shaded part?

owen_sparks

Hi.  @tom_seibold

It's possible to hide anything that is in the way of what you want to focus on.  Either with the "eye" icon to the right of parts and some features in the tree on the left pane of the screen, or via the right click context sensitive menu, or by pressing the "Y" key when hovering over something in the modeling area.

Also just a friendly nudge to post a link to your document as mentioned above, we could have saved you a bit of time

Cheers, and Happy CADing,

Owen S.

tom_seibold

@owen_sparks The eye icon doesn't appear on extrudes, fillets, and holes (in the Features list) that make up my model. It does appear on sketches, but it appears any sketch that is not currently being edited is visibility-off (line through eye) by default--at least in my file. I do appreciate you making me aware of the hide command in its various manifestations, but that's not solving the problem for me, either. When I hide the extruded part my type sketch is attached to (Part 1), I see a white background. Success! But, no: As soon as I double-click Sketch 15 (the sketch containing the mostly imported logo) to edit it, the background the letters appear are on becomes shaded along with the letters themselves, so I still can't check for open regions! Now, I see that the circle around the letters (edges of the formerly visible Part 1) is highlighting on mouseover, so perhaps it is also a closed region that's shading when the sketch is edited. But it's not one that I drew, so I'm not sure how to hide it. Here's the link if you'd like to inspect: https://cad.onshape.com/documents/699a9674479007024e599743/w/0a6ed61b4075b75b2f5b36a2/e/4fb5d462993aa511cef60aee

bruce_williams

@tom_seibold

Well, kudos to you for working on analyzing this!  What you are seeing is the shading of the face you chose to create sketch 15.  Hopefully an Onshape guru (@NeilCooke) will chime in with a way to hide that shading as I do not know how.  Normally it is not a problem but you are trying to fix imported geometry.

One good work around is to create a new plane (use 0 offset to your face).  Create sketch on that plane to import the geometry.  That will give you a simple sketch with only the import and not the background shaded.  

owen_sparks

Hi @tom_seibold

Looks like you got it fixed before I saw your new post

(1) So the behaviour you describe of the hidden part being shown in your sketch is described by Onshape as "imprinting".  Sometimes it's useful, other times like this not so much. 

There is a way to defeat it though. 
In this file I've added a new plane in the feature tree just before the problem sketch and then moved your sketch exactly as it was but onto the new plane. (Sketches on parts allow imprinting, sketches on planes do not.)
https://cad.onshape.com/documents/d63feee0701f9c08c3e8d78d/v/34c7dbfa510ee16c2440b54c/e/9033d071c97ab5bd861832ed
This means your sketch will appear as in video @bruce_williams posted.

There is an improvement request here that would make this imprinting optional, should you care to cast your vote:-
https://forum.onshape.com/discussion/comment/46677

(2) Just an an FYI if you use the share option to get a link and then post that on the forum that only gives us a read only link we can't copy or edit.  It makes our life easier if you just copy the url straight from the browser.

(3) It's really helpful if you're intending to carry on working whilst you have an open question on the forum if you throw a revision of the document and then link to that on the forum.  (That way you can carry on working in the "main workspace" and we can see your document frozen in time when the problem arose.  If you click on the link for my copy you'll see it at Rev2, but I'm free to carry on doing other work on it if need be.

Feel free to shout with any questions, it's a friendly place here.
Cheers, Owen S.

owen_sparks

Grrr @bruce_williams looks like our posts crossed in the ether.   

bruce_williams

@owen_sparks
Quite alright!  You have a much better and fuller explanation.  I learned a couple of things.  

And aren't you in Europe?  Staying up late on Onshape forum heh?  

owen_sparks

Hi Bruce.  Yeah, I'm in Wales in the UK but it's not too late yet.  Had a frustrating day with a Microsoft product so it was nice to pop back onto the forum and actually be able to answer something    Maybe we should set up some sort of a rota though, or we could just let @john_mcclary answer everything, I'm just about convinced that bloke is imunue to sleep.

tom_seibold

@owen_sparks Great tip on the new-plane technique to overcome the imprinting--I appreciate the acknowledgment that the shading problem was not just my imagination! Your point 2: I could swear that what I did WAS copy and paste the browser URL--not sure why it didn't work. So how were you able to create a copy for testing? Your point 3: Another good tip--I must use versioning more.

john_mcclary

owen_sparks said:

I'm just about convinced that bloke is imunue to sleep.

Sleep... meh... that's just 3-1/2 hours a night wasted not browsing the forums...

By the way, you don't need to create a new plane anymore to avoid imprinting.
You can use the implied mate connector in the sketch creation instead... save a step

owen_sparks

@tom_seibold
Sure thing.
(1) Was a take-away from a webinar @philip_thomas hosted concerning good modelling practices, specifically modelling for good rebuild performance.  Just about anything that chap says is worth listening too but he feels the urge to jump out of perfectly good aeroplanes from time to time so he's a bit strange.  He's been a bit quiet recently; you OK Philip?

(2) Might just have been me.  If you can see the title of the document in something read-only then you can go to the "public" bit of "MyOnshape" and then search for the file.  Works well unless the author has called the document something like "Testing"!

(3) Also branching. Branching is even better for helping.  Still waiting patiently for Onshape to allow sharing just a branch of a document not the whole thing.  That way it would be safe to work in the actual document not a copy of a copy. 

Cheers, Owen.  Off in search of lunch...

owen_sparks

john_mcclary said:

owen_sparks said:

I'm just about convinced that bloke is imunue to sleep.

Sleep... meh... that's just 3-1/2 hours a night wasted not browsing the forums...

By the way, you don't need to create a new plane anymore to avoid imprinting.
You can use the implied mate connector in the sketch creation instead... save a step

That's clever.  Thanks; see we're all learning stuff...
Right, forum off, lunch in.  I can do that, maybe.

philip_thomas

@owen_sparks -

• I am alive and well - thank you
• Thank you for being active on these forums (as so many of you are)
• Yes, the dividing line technique has yet to be surpassed in either speed or efficiency
• The 'make plane' prior to sketching is the best way to prevent imprinting (the mate connector plane hack is a nice click saver)
• If you (plural) want the option to suppress imprinting on sketch creation, we have a story (Onshape unit of work) for it and are collecting votes - so vote!

What am I doing? I am involved in a lot of projects surrounding the integration with PTC (the company, not any specific product).
Its going well and the goal is absolutely to deliver more capabilities faster!
PTC has made a big bet on us and we intend to deliver.

Jake_Rosenfeld

Us software people justify the "line dividing technique" by calling it a "binary search" and asserting that it takes log(n) time (where n would be the amount of time it took to just check every vertex to see if its actually connected).

People like Philip in the company tend to respond, "That's just a clever excuse to avoid making a tool that finds or fixes these cases automatically."

To each their own I guess 

philip_thomas

Users: If you want this tool (automatic highlighting of non contiguous edges), submit enhancement requests - nothing has changed, we work on whatever is at the top of the list!

Also - we moved into our new building last week - this a small sample of our 360 degree view of Boston - anyone is welcome to visit us at any time (this is from the 13th floor - there are 17 floors).