AnsweredAssumed Answered

Surface to Solid Feature?

Question asked by robert dattilo on Apr 17, 2012
Latest reply on Oct 2, 2018 by Shawn Stugard

Like • Show 1 Like1
Comment • 16

Hello;

I know that it's possible to create a solid from a surface, but was wondering if you can, & if so,

what would be the best way to go about creating a surfaced feature, & then blending or converting that to a solid

feature?

I usually just work in solids, but someone wants a bit of a tricky feature, that looks like it would

just be alot easier to construct with the surface tools, but the rest of the models features are in solids.

Anyone know the best way to approach this?

Thanks, in advance;

Rob_D SW 2012 sp1

Dwight Livingston Apr 17, 2012 11:22 AM

Correct Answer

You can either use Knit (if you have a complete set of surfaces)

or Fill Surface (if you have one surface body with a missing face).

See the reply in context

No one else had this question

Outcomes

16 Replies

Dwight Livingston Apr 17, 2012 11:22 AM
Unmark Correct
Correct Answer
You can either use Knit (if you have a complete set of surfaces)

or Fill Surface (if you have one surface body with a missing face).
Like • Show 4 Likes4
Actions
- Dwight Livingston @ Dwight Livingston on Apr 17, 2012 11:25 AM
  Mark Correct
  Correct Answer
  Or, should you somehow create a closed and knit surface body, you can use a Delete Face with a Delete and Fill to create the soild body.
  Like • Show 4 Likes4
  Actions
  - Ahmet Ozgur Ergin @ Dwight Livingston on Apr 5, 2017 7:50 AM
    Mark Correct
    Correct Answer
    Thanks for the tip.
    Like • Show 1 Like1
    Actions
  - Shawn Stugard @ Dwight Livingston on Mar 27, 2018 2:17 PM
    Mark Correct
    Correct Answer
    I forgot all about this method, thanks!
    Like • Show 1 Like1
    Actions
- robert dattilo @ Dwight Livingston on Apr 19, 2012 11:32 AM
  Mark Correct
  Correct Answer
  Hello Dwight;
  
  Yeah, that worked great. Since I was attaching a feature to like a cylindrical feature, I did have to fill the cylinder side of the new surface group. That enabled the form solid option, to work. It then listed it under the solid bodies.
  
  Thanks for the tip;
  
  Rob_D SW 2012 sp1
  Like • Show 1 Like1
  Actions
Chris Kamery Apr 19, 2012 11:46 AM
Mark Correct
Correct Answer
Robert,

Another method is that once all of the surfaces have been made and knitted together, the Thicken Tool can be also used.

I got tripped up once on a certification exam that asked how to make a solid from a surface and I got it wrong because I didnt say Thicken. As you can see there is more than one solution as well.

Chris
Like • Show 2 Likes2
Actions
- Dwight Livingston @ Chris Kamery on Apr 19, 2012 1:26 PM
  Mark Correct
  Correct Answer
  Chris
  
  Didn't know about that. Thanks. That is certainly better than using a Delete Face.
  
  When _is_ one likely to get a closed and knitted surface body, when what you want is a solid body?
  
  Dwight
  Like • Show 1 Like1
  Actions
  - Chris Kamery @ Dwight Livingston on Apr 20, 2012 8:12 AM
    Mark Correct
    Correct Answer
    Dwight,
    
    I cannot say I have run into the situation often. Maybe once or twice on an imported part. Generally I try to form a solid using the knit command. If it will knit but not form a solid, chances are Thicken would fail as well. Matt or Charles may have some examples of which they had a single surface body enclosing a volume and would then just need to be converted to a solid.
    
    Chris
    Like • Show 1 Like1
    Actions
    - Dwight Livingston @ Chris Kamery on Apr 20, 2012 9:17 AM
      Mark Correct
      Correct Answer
      Chris Kamery wrote:
      
      . . . Matt or Charles may have some examples of which they had a single surface body enclosing a volume and would then just need to be converted to a solid. . .
      Yeah, I'm curious. SW did put some work into that Thicken option, which only comes up if you select a closed surface body.
      Like • Show 1 Like1
      Actions
      - Jerry Steiger @ Dwight Livingston on Apr 30, 2012 8:39 PM
        Mark Correct
        Correct Answer
        Dwight,
        
        I have had Knit fail to make a solid body several times. I've had Thicken work after Knit failed on a couple of them. I have no idea why. I just count my blessings and try not to look a gift horse in the mouth!
        
        Jerry Steiger
        Like • Show 1 Like1
        Actions
        Dwight Livingston @ Jerry Steiger on Apr 30, 2012 10:05 PM
        Mark Correct
        Correct Answer
        Jerry
        
        Good to know that. We all need a card up the sleeve at times.
        
        Thanks
        
        Dwight
        Like • Show 1 Like1
        Actions
        Jason Swackhamer @ Jerry Steiger on May 1, 2012 9:05 AM
        Mark Correct
        Correct Answer
        Jerry-
        
        Hope I'm not going off on too much of a tangent, but this is something I find increasingly annoying with solidworks--one method works and another doesn't. This has always been a problem, but as the methods for creating solids proliferate, so do the workarounds. I ran into this recently when using the mold tools. The tooling split wouldn't work, but extruding a solid up to a knitted surface of the core and parting line did. This was a few days ago, but I think the error message was something like "Unable to knit surfaces into a solid".
        
        Now here's the interesting thing, after trying a gazillion different "fixes" for the tooling split problem, I ran a check part and discovered there was a general fault error in the model which only showed up with the "stringent solid/surface check" checkbox checked. Once I fixed that, the part split fine.
        
        So it seems that the tooling split function uses more thorough error checking than boss extrude (which kind of makes sense, I guess), but instead of giving me a "what's wrong" message that pertains to the actual error it found, it gives me a useless boiler plate message. I mean how difficult would it be to say something like "Unable to complete operation due to a general fault in the model"?
        
        Anyway, reading through this thread put me in mind of this growing source of frustration...
        
        -Jason S.
        Like • Show 2 Likes2
        Actions
        Jerry Steiger @ Jason Swackhamer on May 8, 2012 10:19 PM
        Mark Correct
        Correct Answer
        Jason,
        
        I have also seen cases where a part that fails a check will not allow a feature, where the same part after fixing the "original" geometry problem will allow a feature. I too have seen any number of seemingly meaningless error messages and get very frustrated with them. I do cut the guys writing the code a little slack, though, because it must be really hard to come up with messages covering all of the many possible problems that make sense to users who don't know anything about the way the code actually works.Still, it seems like sometimes they are just pulling them out of fortune cookies!
        
        Jerry Steiger
        Like • Show 1 Like1
        Actions
  - Jeff Root @ Dwight Livingston on Feb 3, 2016 3:15 AM
    Mark Correct
    Correct Answer
    Dwight,
    Thanks for the tip on Delete Face using the Delete and Fill option to create a solid body, I just used this and it worked well.
    You asked when it is likely to be working from a closed and knitted surface body, when you want a solid body. I just encountered this, so I'll tell you my case:
    Im creating a new part in an assembly that has in-context surface relationships with a pre-existing part within the assembly. The first feature within the new part started with a Surface-Offset (value of 0.000) command that referenced certain surfaces from the parent part. These offset surfaces formed a closed, knitted complete surface, with no option at that point to make a solid body. From there I used your trick of choosing one face to Delete and Fill to create the solid.
    Thanks!
    Jeff
    Like • Show 1 Like1
    Actions
Chris Pratt Apr 11, 2018 1:23 PM
Mark Correct
Correct Answer
For those lost souls on google, SolidWorks 2013 and later also has "Insert -> Features -> Intersect" for turning surfaces into a solid.
Like • Show 3 Likes3
Actions
- Shawn Stugard @ Chris Pratt on Oct 2, 2018 2:28 PM
  Mark Correct
  Correct Answer
  Love this feature, big time saver when knit and/or combine are not doing the trick.
  Like • Show 0 Likes0
  Actions

Surface to Solid Feature?

Outcomes

Related Content

Recommended Content

Incoming Links