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3D Sketch, Helices, and Composite curve...

Question asked by Guy Veber on Jul 7, 2010
Latest reply on Jul 10, 2010 by 1-4EQZK9

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I am creating an incandescent fluorescent light bulb.

And my idea was to create two helices intertwined and then use 3D sketch to connect the top of the helices together using a 3D spline, and connecting the two bottom helices to the base of the bulb using a similar 3D spline. I would then create a composite curve by selecting all four entities (2x helices, 3x 3D splines) to make one complex curve. Then create a circle at the end of the complex curve to be used as the profile for a sweep to create the fluorescent tube bulb for the incandescent light bulb.

However when I try to create the composite curve the relations added to the helices and splines give errors that there are discontinuity between the helices and 3D sketched splines. The relations that are available when I created the 3D splines to the helices are only tangent and equal curvature.

I am stuck and not sure why the 3D sketch does not work when making this, it seems to be a simple composite curve?

1-4EQZK9 Jul 8, 2010 10:25 PM

Correct Answer

Hi Guy, (hum - that sounds kinda strange...)

Take a look at the example attached. You are almost there. SW Sweep is a bit fussy about multiple connected sketch entities and the shape that results. The key to most of these type of issues is: Fit Spline. What I did:

1) create 2 helix curves 180 degrees from one another

2) create a single 3D sketch that connects the top ends and finishes the bottoms of the tube.

3) DO A SINGLE FIT SPLINE thru all sketch entities and the two helix curves. (no need to convert entities on the helix.)

4) create your tube diameter and sweep.

Best Regards

Mark

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Incandescent Fluorescent Lightbulb.JPG41.6 KB

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1-4EQZK9 Jul 8, 2010 6:59 AM

Guy,

Post your part so we can see what you are describing. BTW, there is little need to create composite curves anymore since there is the SelectionManager for Sweep (and other surface features.)

thanks

Mark

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Guy Veber @ 1-4EQZK9 on Jul 8, 2010 1:57 PM

So my next course of action was a suggestion by Matt Lombard.

Convert the helices to splines via the 3d sketch. Meaning I edited the 3D sketch which had the 3x 3D splines connecting the base of the lightbulb to the helices, I then converted the helices to splines and added the needed relations (tangency, and coincidence) however my sweep will not complete as there are intersecting problems now, it seems as there are small kinks at the base where I used two 3D splines to connect to the original helices.

However I am still unable to complete the sweep despite clicking on on every available option in the sweep command.

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Flourescent Lightbulb.JPG39.6 KB

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Harold Brunt Jul 8, 2010 1:35 PM

Guy,

Are you trying to model a compact fluorescent bulb by any chance? Typically a bulb is either an incandescent or a fluorescent, not both. Can you tell us what you are up to or email me directly and tell me what you can? I'm certainly intrigued.

Harold

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Roland Schwarz Jul 8, 2010 4:37 PM

You're making it a tad too difficult. Once you make the helices, make a single 3D sketch to connect them, including using Convert Entities to bring copies of the helices right into the 3D sketch. Use the 3D sketch to construct your sweep. No need for the extra step of the composite curve.

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Guy Veber @ Roland Schwarz on Jul 8, 2010 6:16 PM

I agree having 3 sketches for a single item each would be redundant. So to answer your question there is only one 3D sketch with 3x splines. One spline connects the two helices at the top, and the other two splines connect the helices to the base of the bulb. Now I currently edited the 3D sketch and converted the two helices to splines as well, so now the Sweep see's the 3D sketch continuous for the path.

Now I can create a composite curve, or use the newly converted splines to be used for my path. However now I get errors, "The Sweep could not complete itself because it intersected itself while passing through segment #1 of the path". This has to be one of the two splines at the bottom connecting the helices to the bulb base. As I look closer at the model there is some inconsistency with the sweep as it seems to kink and does not make a fluid sweep as I would like, (this is the preview as the sweep will not complete). I have manipulated the handles on the splines but I can't seem to find a happy medium.

So my guess is that the relations of tangent and equal curvature do not really work well in this scenario. I thought the composite curve would solve my issue here, but Roland you are right as Matt Lombard told me earlier it's not really needed after I converted the helices to splines in the 3D sketch.

I have posted a picture it includes my build order so you can see my progression. I am open for any suggestions as I am trying to improve my skill set and I am sure there are many ways to do this.

Attachments

Fluorescent Lightbulb #2.JPG66.0 KB

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1-4EQZK9 @ Guy Veber on Jul 8, 2010 10:25 PM

Hi Guy, (hum - that sounds kinda strange...)

1) create 2 helix curves 180 degrees from one another

2) create a single 3D sketch that connects the top ends and finishes the bottoms of the tube.

3) DO A SINGLE FIT SPLINE thru all sketch entities and the two helix curves. (no need to convert entities on the helix.)

4) create your tube diameter and sweep.

Best Regards

Mark

Attachments

CFL-mab.SLDPRT.zip762.6 KB

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Guy Veber @ 1-4EQZK9 on Jul 8, 2010 11:42 PM

Thank you Mark,

That did the trick... I have not used the fit spline command before I usually manipulate the handles, but that tool is even more impressive as it converted all the bodies into one curve for the path.

Awesome...

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Guy Veber @ 1-4EQZK9 on Jul 9, 2010 9:19 PM

Why is it, the spline is so picky? Half the time "Fit Spline" works and the sweep can be created, the other half, I have to sit there a mess with it to get it to work.

I don't understand why there isn't a simple way to do this. If the spline up top isn't just so, there are a number of different errors to be had. So why is that? what are the relations that need to be to make the spline work?

Also is that the sweep doesn't like kinks, I ask because one of the bigger errors I get is that the sweep or spline will be self intersecting. And despite my geometry does not show that there may be a turn which is not exactly smooth and rounded but more of a 100 degree bend.

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1-4EQZK9 @ Guy Veber on Jul 10, 2010 6:35 PM

Hi Guy,

Sweeping problems generally occur when the path is 3D and the sweep profile needs to understand how to traverse the path and how to position the profile relative to the path (default normal.) In some cases just sweeping the path normal to every point in the path will not give you the desire solution. Did you notice that I turned on the option "minimum twist"? - this usually elevates the problems associated with "knots" ( intersections between sketch entities or interim spline points.)

I have notice one bug with our fit spline and your example part; if you delete the fit spline and then recreated it it sometimes won't work because after deleting the previous fit spline, it turn all of the underlying geometry (helix curve and 3D curves etc.) to construction geometry. Well, it sometimes won't fit over construction geometry so you have to toggle it back to geometry and then it will work.

Yes, this is an art, but with a little practice and knowledge, - you'll be a pro and have a lot more power and versatility modeling.

Regards

Mark

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9 Replies

1-4EQZK9 Jul 8, 2010 6:59 AM
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Correct Answer
Guy,

Post your part so we can see what you are describing. BTW, there is little need to create composite curves anymore since there is the SelectionManager for Sweep (and other surface features.)

thanks

Mark
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- Guy Veber @ 1-4EQZK9 on Jul 8, 2010 1:57 PM
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  Correct Answer
  So my next course of action was a suggestion by Matt Lombard.
  Convert the helices to splines via the 3d sketch. Meaning I edited the 3D sketch which had the 3x 3D splines connecting the base of the lightbulb to the helices, I then converted the helices to splines and added the needed relations (tangency, and coincidence) however my sweep will not complete as there are intersecting problems now, it seems as there are small kinks at the base where I used two 3D splines to connect to the original helices.
  
  However I am still unable to complete the sweep despite clicking on on every available option in the sweep command.
  Attachments
  - Flourescent Lightbulb.JPG39.6 KB
  Like • Show 0 Likes0
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Harold Brunt Jul 8, 2010 1:35 PM
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Correct Answer
Guy,

Are you trying to model a compact fluorescent bulb by any chance? Typically a bulb is either an incandescent or a fluorescent, not both. Can you tell us what you are up to or email me directly and tell me what you can? I'm certainly intrigued.

Harold
Like • Show 0 Likes0
Actions
Roland Schwarz Jul 8, 2010 4:37 PM
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Correct Answer
You're making it a tad too difficult. Once you make the helices, make a single 3D sketch to connect them, including using Convert Entities to bring copies of the helices right into the 3D sketch. Use the 3D sketch to construct your sweep. No need for the extra step of the composite curve.
Like • Show 0 Likes0
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- Guy Veber @ Roland Schwarz on Jul 8, 2010 6:16 PM
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  Correct Answer
  I agree having 3 sketches for a single item each would be redundant. So to answer your question there is only one 3D sketch with 3x splines. One spline connects the two helices at the top, and the other two splines connect the helices to the base of the bulb. Now I currently edited the 3D sketch and converted the two helices to splines as well, so now the Sweep see's the 3D sketch continuous for the path.
  
  Now I can create a composite curve, or use the newly converted splines to be used for my path. However now I get errors, "The Sweep could not complete itself because it intersected itself while passing through segment #1 of the path". This has to be one of the two splines at the bottom connecting the helices to the bulb base. As I look closer at the model there is some inconsistency with the sweep as it seems to kink and does not make a fluid sweep as I would like, (this is the preview as the sweep will not complete). I have manipulated the handles on the splines but I can't seem to find a happy medium.
  
  So my guess is that the relations of tangent and equal curvature do not really work well in this scenario. I thought the composite curve would solve my issue here, but Roland you are right as Matt Lombard told me earlier it's not really needed after I converted the helices to splines in the 3D sketch.
  
  I have posted a picture it includes my build order so you can see my progression. I am open for any suggestions as I am trying to improve my skill set and I am sure there are many ways to do this.
  Attachments
  - Fluorescent Lightbulb #2.JPG66.0 KB
  Like • Show 0 Likes0
  Actions
  - 1-4EQZK9 @ Guy Veber on Jul 8, 2010 10:25 PM
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    Correct Answer
    Hi Guy, (hum - that sounds kinda strange...)
    
    Take a look at the example attached. You are almost there. SW Sweep is a bit fussy about multiple connected sketch entities and the shape that results. The key to most of these type of issues is: Fit Spline. What I did:
    
    1) create 2 helix curves 180 degrees from one another
    2) create a single 3D sketch that connects the top ends and finishes the bottoms of the tube.
    3) DO A SINGLE FIT SPLINE thru all sketch entities and the two helix curves. (no need to convert entities on the helix.)
    4) create your tube diameter and sweep.
    
    Best Regards
    
    Mark
    Attachments
    CFL-mab.SLDPRT.zip762.6 KB
    Like • Show 0 Likes0
    Actions
    - Guy Veber @ 1-4EQZK9 on Jul 8, 2010 11:42 PM
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      Correct Answer
      Thank you Mark,
      
      That did the trick... I have not used the fit spline command before I usually manipulate the handles, but that tool is even more impressive as it converted all the bodies into one curve for the path.
      
      Awesome...
      Like • Show 0 Likes0
      Actions
    - Guy Veber @ 1-4EQZK9 on Jul 9, 2010 9:19 PM
      Mark Correct
      Correct Answer
      Why is it, the spline is so picky? Half the time "Fit Spline" works and the sweep can be created, the other half, I have to sit there a mess with it to get it to work.
      I don't understand why there isn't a simple way to do this. If the spline up top isn't just so, there are a number of different errors to be had. So why is that? what are the relations that need to be to make the spline work?
      
      Also is that the sweep doesn't like kinks, I ask because one of the bigger errors I get is that the sweep or spline will be self intersecting. And despite my geometry does not show that there may be a turn which is not exactly smooth and rounded but more of a 100 degree bend.
      Like • Show 0 Likes0
      Actions
      - 1-4EQZK9 @ Guy Veber on Jul 10, 2010 6:35 PM
        Mark Correct
        Correct Answer
        Hi Guy,
        
        Sweeping problems generally occur when the path is 3D and the sweep profile needs to understand how to traverse the path and how to position the profile relative to the path (default normal.) In some cases just sweeping the path normal to every point in the path will not give you the desire solution. Did you notice that I turned on the option "minimum twist"? - this usually elevates the problems associated with "knots" ( intersections between sketch entities or interim spline points.)
        
        I have notice one bug with our fit spline and your example part; if you delete the fit spline and then recreated it it sometimes won't work because after deleting the previous fit spline, it turn all of the underlying geometry (helix curve and 3D curves etc.) to construction geometry. Well, it sometimes won't fit over construction geometry so you have to toggle it back to geometry and then it will work.
        
        Yes, this is an art, but with a little practice and knowledge, - you'll be a pro and have a lot more power and versatility modeling.
        
        Regards
        
        Mark
        Like • Show 0 Likes0
        Actions

3D Sketch, Helices, and Composite curve...

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