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Create Part From Swept Cut Sketch..........Within The Part........ Possible????

Question asked by Dave Bear on May 10, 2017
Latest reply on May 11, 2017 by Dan Pihlaja

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Hi All,

Okay, so here's the scenario. If you look at the attached part you'll notice that I created two sketches on different planes that were fully defined. These two sketches do however have two common intersections. I then used a third sketch in 3D mode and just simply converted all of the entities from the previous two sketches to end up with my complete 3D sketch. I then used this 3D sketch as the path for a 3mm Swept Cut in the base of the part. * Doing this whole process was far easier and quicker than trying to do just one 3D sketch and fully defining it*

The Swept Cut in the base of the part is for a seal made from O-ring material. What I want to know now is can I use this 3D sketch and make my seal now within this part and then save it as a separate part? i.e. "The Seal".

Obviously this would be a Swept Boss/Base and it would not be merged. But can it be done and what are the proper steps?

Dave.

Bjorn Hulman May 10, 2017 7:58 AM

Correct Answer

Hi Dave,

Yes you can sweep around your 3D sketch, if you really want you can use the same profile as the cut as well. Ensure merge result is off. In the feature tree, expand the solid bodies folder, right click the sweep body and select 'insert into new part'

EDIT,

been working in SW2014 until this week, the new circular profile functionality is a winner!!

See the reply in context

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X2 - Rocker Cover (Right).SLDPRT.zip753.0 KB

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Bjorn Hulman May 10, 2017 7:58 AM

Hi Dave,

EDIT,

been working in SW2014 until this week, the new circular profile functionality is a winner!!

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Dave Bear @ Bjorn Hulman on May 10, 2017 8:06 AM

Cheers Bjorn,

I'll give it a crack in a few minutes and let you know the outcome..............

Dave.

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Dave Bear @ Bjorn Hulman on May 10, 2017 8:45 AM

It does work Bjorn, but with some issues.

It creates a new part as you indicated, but it is linked to the original part and I cannot find an option to break it.

If I create the new part and save it as it's own entity and then go back to the original and delete the Swept Boss, the new part when re-opened basically becomes a copy of the original part that the seal was created from and there is no evidence of a seal in either part file.

I can suppress the Swept Boss after the new part is created and saved I guess but I really wish it had no links or references to anything.

Any idea?

*** EDIT *** I can't even suppress the Swept Boss as this then makes the new part (seal) turn into a complete copy of the rocker cover part.......... Crazy!!!!!!

Dave.

Attachments

X4 - Rocker Cover Seal (Right).sldprt.zip161.4 KB

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Bjorn Hulman @ Dave Bear on May 10, 2017 8:47 AM

Hi Dave,

There's a few things you can do there

in the new part, right click the feature and select 'List external references' and select lock all. That would give you the option of unchecking it if you make changes.

Otherwise, you could start a new part, expand the file explorer tab on the right of the interface, Open in Solidworks, drag the X2... part in. unselect all boxes other than the absorbed sketches box. and click ok. In the feature tree expand it out and you'll have the 3D sketch at the bottom, then you can sweep. This will remain linked to the original.

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Bjorn Hulman @ Bjorn Hulman on May 10, 2017 8:49 AM

I'd probably go with the'otherwise' direction

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Dave Bear @ Bjorn Hulman on May 10, 2017 8:54 AM

Hey Bjorn,

I've found where to break the link to external references. In the new part, I RMB on the new part in the Feature Tree "Stock - X2....." and then selected List External Refs from there. There was an option the to break them. Before I was looking at the 'Edit' and File' options on the main screen and trying to do it from there.

All good now buddy............ Thank you so much for your time and help!

Dave.

Actions

Dan Pihlaja May 10, 2017 9:37 AM

Dave Bear wrote:

Hi All,
Okay, so here's the scenario. If you look at the attached part you'll notice that I created two sketches on different planes that were fully defined. These two sketches do however have two common intersections. I then used a third sketch in 3D mode and just simply converted all of the entities from the previous two sketches to end up with my complete 3D sketch. I then used this 3D sketch as the path for a 3mm Swept Cut in the base of the part. * Doing this whole process was far easier and quicker than trying to do just one 3D sketch and fully defining it*

The Swept Cut in the base of the part is for a seal made from O-ring material. What I want to know now is can I use this 3D sketch and make my seal now within this part and then save it as a separate part? i.e. "The Seal".
Obviously this would be a Swept Boss/Base and it would not be merged. But can it be done and what are the proper steps?

Dave.

Another option is to create a temporary assembly.....then add your part with your first two sketches into it. Then add a 2nd empty part.

When you create your 3d sketch, first edit the 2nd part in context in the assembly, then create a 3d sketch in there, and convert all the entities from the 2 sketches in the first part. However, make sure that "No External References" is turned on.

After you have created your 3D sketch, exit the sketch, exit the in context editing and then just open the 2nd part separately and do your sweeps. Maybe you want to edit the sketch and add relations to it first though.

Then you can delete your assembly.

Actions

Dave Bear @ Dan Pihlaja on May 11, 2017 5:34 AM

Hi Dan,

Thanks for the tip! You've also highlighted a little feature (command box) that I've never seen before. Might need to add that one to my toolbar.

Dave.

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Dan Pihlaja @ Dave Bear on May 11, 2017 8:44 AM

That is only available when you are in an assembly and editing a part in context.

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Dave Bear @ Dan Pihlaja on May 11, 2017 8:49 AM

Oh okay.......

I've got to try a similar process in the next couple of days so I'll give your method a crack and see how badly I can stuff it all up lol.

I'll let you know how I go.......

Dave.

Actions

Dave Bear @ Dan Pihlaja on May 11, 2017 9:21 AM

Thank you Dan,

I appreciate the links, no doubt I'll get confused somewhere so they're bound to come in handy!

Dave.

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Dan Pihlaja @ Dave Bear on May 11, 2017 9:57 AM

No problem....

All those people who spend the time to write those articles and post them where they are part of the public domain....

Those people are my friends.... They don't know it.....but they are.

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13 Replies

Bjorn Hulman May 10, 2017 7:58 AM
Unmark Correct
Correct Answer
Hi Dave,
Yes you can sweep around your 3D sketch, if you really want you can use the same profile as the cut as well. Ensure merge result is off. In the feature tree, expand the solid bodies folder, right click the sweep body and select 'insert into new part'
EDIT,
been working in SW2014 until this week, the new circular profile functionality is a winner!!
Like • Show 3 Likes3
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- Dave Bear @ Bjorn Hulman on May 10, 2017 8:06 AM
  Mark Correct
  Correct Answer
  Cheers Bjorn,
  I'll give it a crack in a few minutes and let you know the outcome..............
  
  Dave.
  Like • Show 1 Like1
  Actions
- Dave Bear @ Bjorn Hulman on May 10, 2017 8:45 AM
  Mark Correct
  Correct Answer
  It does work Bjorn, but with some issues.
  It creates a new part as you indicated, but it is linked to the original part and I cannot find an option to break it.
  If I create the new part and save it as it's own entity and then go back to the original and delete the Swept Boss, the new part when re-opened basically becomes a copy of the original part that the seal was created from and there is no evidence of a seal in either part file.
  
  I can suppress the Swept Boss after the new part is created and saved I guess but I really wish it had no links or references to anything.
  
  Any idea?
  
  *** EDIT *** I can't even suppress the Swept Boss as this then makes the new part (seal) turn into a complete copy of the rocker cover part.......... Crazy!!!!!!
  
  Dave.
  Attachments
  - X4 - Rocker Cover Seal (Right).sldprt.zip161.4 KB
  Like • Show 1 Like1
  Actions
  - Bjorn Hulman @ Dave Bear on May 10, 2017 8:47 AM
    Mark Correct
    Correct Answer
    Hi Dave,
    There's a few things you can do there
    in the new part, right click the feature and select 'List external references' and select lock all. That would give you the option of unchecking it if you make changes.
    Otherwise, you could start a new part, expand the file explorer tab on the right of the interface, Open in Solidworks, drag the X2... part in. unselect all boxes other than the absorbed sketches box. and click ok. In the feature tree expand it out and you'll have the 3D sketch at the bottom, then you can sweep. This will remain linked to the original.
    Like • Show 3 Likes3
    Actions
    - Bjorn Hulman @ Bjorn Hulman on May 10, 2017 8:49 AM
      Mark Correct
      Correct Answer
      I'd probably go with the'otherwise' direction
      Like • Show 1 Like1
      Actions
    - Dave Bear @ Bjorn Hulman on May 10, 2017 8:54 AM
      Mark Correct
      Correct Answer
      Hey Bjorn,
      I've found where to break the link to external references. In the new part, I RMB on the new part in the Feature Tree "Stock - X2....." and then selected List External Refs from there. There was an option the to break them. Before I was looking at the 'Edit' and File' options on the main screen and trying to do it from there.
      
      All good now buddy............ Thank you so much for your time and help!
      
      Dave.
      Like • Show 4 Likes4
      Actions
Dan Pihlaja May 10, 2017 9:37 AM
Mark Correct
Correct Answer
Dave Bear wrote:

Hi All,
Okay, so here's the scenario. If you look at the attached part you'll notice that I created two sketches on different planes that were fully defined. These two sketches do however have two common intersections. I then used a third sketch in 3D mode and just simply converted all of the entities from the previous two sketches to end up with my complete 3D sketch. I then used this 3D sketch as the path for a 3mm Swept Cut in the base of the part. * Doing this whole process was far easier and quicker than trying to do just one 3D sketch and fully defining it*

The Swept Cut in the base of the part is for a seal made from O-ring material. What I want to know now is can I use this 3D sketch and make my seal now within this part and then save it as a separate part? i.e. "The Seal".
Obviously this would be a Swept Boss/Base and it would not be merged. But can it be done and what are the proper steps?

Dave.

Another option is to create a temporary assembly.....then add your part with your first two sketches into it. Then add a 2nd empty part.
When you create your 3d sketch, first edit the 2nd part in context in the assembly, then create a 3d sketch in there, and convert all the entities from the 2 sketches in the first part. However, make sure that "No External References" is turned on.

After you have created your 3D sketch, exit the sketch, exit the in context editing and then just open the 2nd part separately and do your sweeps. Maybe you want to edit the sketch and add relations to it first though.

Then you can delete your assembly.
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- Dave Bear @ Dan Pihlaja on May 11, 2017 5:34 AM
  Mark Correct
  Correct Answer
  Hi Dan,
  Thanks for the tip! You've also highlighted a little feature (command box) that I've never seen before. Might need to add that one to my toolbar.
  
  Dave.
  Like • Show 2 Likes2
  Actions
  - Dan Pihlaja @ Dave Bear on May 11, 2017 8:44 AM
    Mark Correct
    Correct Answer
    That is only available when you are in an assembly and editing a part in context.
    Like • Show 2 Likes2
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    - Dave Bear @ Dan Pihlaja on May 11, 2017 8:49 AM
      Mark Correct
      Correct Answer
      Oh okay.......
      I've got to try a similar process in the next couple of days so I'll give your method a crack and see how badly I can stuff it all up lol.
      I'll let you know how I go.......
      
      Dave.
      Like • Show 0 Likes0
      Actions
      - Dan Pihlaja @ Dave Bear on May 11, 2017 9:16 AM
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        Correct Answer
        Here are a couple of resources:
        
        An Introduction to In-context Part Editing
        Do You Model In Context?
        SOLIDWORKS: Editing Parts in Context and Transparency | CATI Tech Notes
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        Dave Bear @ Dan Pihlaja on May 11, 2017 9:21 AM
        Mark Correct
        Correct Answer
        Thank you Dan,
        I appreciate the links, no doubt I'll get confused somewhere so they're bound to come in handy!
        
        Dave.
        Like • Show 1 Like1
        Actions
        Dan Pihlaja @ Dave Bear on May 11, 2017 9:57 AM
        Mark Correct
        Correct Answer
        No problem....
        
        All those people who spend the time to write those articles and post them where they are part of the public domain....
        
        Those people are my friends.... They don't know it.....but they are.
        Like • Show 1 Like1
        Actions

Create Part From Swept Cut Sketch..........Within The Part........ Possible????

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