AnsweredAssumed Answered

Why Isn't This Tube Continuous?

Question asked by Keaton Warn on Jun 7, 2018
Latest reply on Jun 8, 2018 by Keaton Warn

Like • Show 0 Likes0
Comment • 10

I want this tube coil model to at least appear to be continuous for the purpose of having an accurate view in a drawing file. Notice how the solid body doesn't appear to be continuous.

Helix Settings:

Sweep sketch dimensions:

If I increase the difference between the OD of the tube (0.875) and the pitch (0.8750001) to something as much as 0.0001, it appears the body becomes continuous. However, I would prefer that the geometry reflect my intent perfectly (0.875 OD, 0.875 pitch).

(Note that if the OD = pitch, it doesn't appear that SolidWorks allows the Sweep function to build the body. Maybe this is due to some sort of zero-width geometry or body intersection error - I'm not sure.)

Here's the result of 0.875 OD, 0.8751 pitch:

(0.875 OD, 0.8751 pitch) Helix Settings for Continuous Body:

No one else has this question

Outcomes

10 Replies

Ruben Balderrama Jun 7, 2018 1:43 PM
Mark Correct
Correct Answer
Attach your file
Like • Show 1 Like1
Actions
- Keaton Warn @ Ruben Balderrama on Jun 8, 2018 8:19 AM
  Mark Correct
  Correct Answer
  My bad. Here it is.
  
  EDIT: If you read the thread, I accidentally uploaded a version of the coil file that had dimensions that did not produce the render error. I've attached "Coil Example 2 (Produces Error)" for future readers. This one has the pitch set to 0.8750001 in, which produces the render error. Moving the trailing "1" to the left by one order of magnitude (0.875001 in) makes the error disappear. Thank you for understanding.
  Attachments
  - Coil Example 2 (Produces Error).zip6.3 MB
  - Coil Example.zip2.5 MB
  Like • Show 2 Likes2
  Actions
Dan Pihlaja Jun 7, 2018 2:02 PM
Mark Correct
Correct Answer
Try increasing your image quality settings. See if that takes care of the issue. If it doesn't then the issue is more than likely the fact that the algorithm for creating the geometry is rounding off some numbers and that edge is the result

The other thing to try is to do it with a sweep with a straight line for the path instead (and a specified twist value). See if that gives you a different result.

In the attached file I have a path length that is simply the OD of the tube * 32. Then I put 32 revolutions into the sweep. It seems to work great and is continuous. Takes a while to rebuild, since each revolution actually touches the previous one. SW 2017 file attached.
Attachments
- twistTube.SLDPRT.zip2.6 MB
Like • Show 2 Likes2
Actions
- Keaton Warn @ Dan Pihlaja on Jun 7, 2018 3:01 PM
  Mark Correct
  Correct Answer
  That's pretty neat. I don't like the seams and how there is a seam that shows up on drawings but this is still a good approach.
  
  I've worked with customer STP files that had that seam and found workarounds to get it to disappear on the drawing, but it can be a pain. It's good to have this option if I need it though.
  
  Here's how the seam shows up:
  Like • Show 1 Like1
  Actions
  - Dan Pihlaja @ Keaton Warn on Jun 7, 2018 3:10 PM
    Mark Correct
    Correct Answer
    I assume that you are talking about this seam:
    
    Yes...I hate that as well. You may need to increase your pitch a little to get away from that. When a body intersects itself, Solidworks automatically creates an edge there. I don't know of another way to go about it.
    
    In my model, if I change the length of the straight line to be .875*32.0001, then there is no seam. And there is a measurable gap between the coils of approximately 0.00007mm.
    Looks better:
    Like • Show 1 Like1
    Actions
    - Keaton Warn @ Dan Pihlaja on Jun 7, 2018 4:04 PM
      Mark Correct
      Correct Answer
      Edit: Yes, it's that seam.
      
      Original Message:
      It's the decision between the lesser of two evils. When dealing with the drawings that have had the seam line on them, I would just put a white circle over it so it wouldn't show up on the drawing. The circle wouldn't always want to stay (especially if it is a SW part file and the radius was changed), but it's a doable workaround.
      Like • Show 2 Likes2
      Actions
Glenn Schroeder Jun 7, 2018 2:38 PM
Mark Correct
Correct Answer
Keaton,

I opened your Part and rotated it every which way and don't see that edge. It might just be a graphics glitch on your machine. Have you tried inserting a drawing view yet? It might not show up there. If it does, I know this might cause some people to break out in hives, but you could hide it there and ignore it in the model.
Like • Show 4 Likes4
Actions
Tony Tieuli Jun 7, 2018 2:59 PM
Mark Correct
Correct Answer
I believe that Glenn Schroeder is right.

See, no edges.
Like • Show 2 Likes2
Actions
- Keaton Warn @ Tony Tieuli on Jun 7, 2018 4:01 PM
  Mark Correct
  Correct Answer
  Glenn and Tony: I just downloaded the .zip I uploaded and I had the pitch at 0.8751, and that does not manifest the render error. The render error isn't manifested until the one is moved ten millionths' place, at 0.8750001. That is my mistake for not double checking the file before I uploaded it.
  
  I went to a different workstation on the LAN and opened the same file and the render error was reproduced.
  
  For now I will just leave it at 0.XXX001, since that does not produce the render error and my assembly isn't that sensitive anyway.
  Like • Show 2 Likes2
  Actions
Keaton Warn Jun 8, 2018 8:22 AM
Mark Correct
Correct Answer
I attached the error-producing file for you guys and for future users to access. Hope something good comes out of it. Hopefully the SolidWorks devs find a way to make it computationally less demanding and more geometrically accurate to model coils in the future.

Thanks for all of the suggestions guys.
Like • Show 1 Like1
Actions

Why Isn't This Tube Continuous?

Outcomes

Attachments

Attachments

Related Content

Recommended Content