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AIRMAN_DILLARD12-Amethyst
12-Amethyst
March 29, 2024
Question

CREO 10 SWEPT BLEND ON A CURVED SURFACE

  • March 29, 2024
  • 3 replies
  • 6510 views

CREO 10

 

CAN YOU COMPLETE A SWEPT BLEND (OR ANOTHER WAY IF THIS IS NOT THE CORRECT FEATURE) FROM A PLANER SKETCH TO A CURVED SKETCH, OR PROJECTED SKETCH ON A CURVED SURFACE?

 

HIGHLIGHTED IS THE PROJECTED SKETCH ON THE LARGE BODY, THE CURSER (SMALL RED LINE) IS THE OUTSIDE SKETCH OF THE DUCT.  FOR THE DUCT, I MADE THE BODY WITH A SWEPT BLEND.  HOWEVER, I NEED TO ADD AN OUTSIDE THICKNESS LAYER WHICH WILL STOP AND CONFORM TO THE OUTTER SURFACE PROFILE OF THE LARGE BODY.  SO BASICALLY, I NEED TO CREATE A LOCATION STOP/SUPPORT FOR THE DUCT (THIS IS REASON I NEED TO ADD EXTERIOR THICKNESS TO THE DUCT), THIS WILL ALLOW ME TO PRINT THIS SEPERATE (IN A DIFFERENT COLOR) AND ASSEMBLE IT TO THE LARGE BODY.  IT IS CRUCIAL FOR ITS LOCATION AFTER ASSEMBLY.

 

I CANNOT PERFORM ANOTHER SWEPT BLEND FOR THE EXTERIOR TO CREATE THE THICKNESS BECAUSE THE SWEEP WILL NOT STOP AT THE CURVED SURFACE.  WHAT ELSE CAN I TRY??

 

ANY HELP IS APPRECIATED.

3 replies

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
March 29, 2024

Are you able to offset the swept surface to the desired thickness? If so then you can offset the swept blend and then trim/merge the proximal and distal ends with surfaces to get a closed quilt that in theory would solidify. Basically, overbuild the geometry with surfaces and trim/merge to get the desired result.

 

You could also get this done with multibody solids and Boolean operations.

 

As with most geometry in Creo there are multiple solutions. Design intent should be a consideration in addition to accurate geometry.

A
AIRMAN_DILLARD12-AmethystAuthor
12-Amethyst
March 29, 2024

HERE'S ANOTHER PICTURE, THE DUCT GOES THROUGH THE BODY A SHORT DISTANCE TO THE INSIDE, THIS NEEDS TO STAY AT THE OUTER DIMENSION TO FIT THROUGH THE OPENING.  WHAT I NEED IS TO THICKEN THE DUCT ON THE OUTSIDE OF THE LARGE BODY.  I NEED THE INCREASED THICKNESS OF THE DUCT TO STOP AT THE CURVED SURFACE OF THE ABUTMENT JOINT AT THE LARGE BODY.  I'VE TRIED RE-SWEEPING THE PROFILE AS A SURFACE AND THEN TRIMMING AND THICKENING BUT I JUST CAN'T GET TO WORK.

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
March 29, 2024

With this extension inside the large body, it would not change my suggestion above. As you build this geometry using surface modeling you should check that it can thicken to the required amount without failure. If you build it with solid geometry, then you could shell it to the required thickness while removing the proximal and distal face surfaces. The corner radii appear to be the limiting factor in terms of achieving the thickness offset. Without access to the geometry, I am speculating. I do not have Creo 10 installed, only up to 9 at the moment.

 

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    achirila5-Regular Member
    5-Regular Member
    April 3, 2024
    Hi @AIRMAN_DILLARD 
    It looks like you have some responses from some community members. If any of these replies helped you solve your question please mark the appropriate reply as the Accepted Solution. 
    Of course, if you have more to share on your issue, please let the Community know so other community members can continue to help you.
    tbraxton
    22-Sapphire II
    tbraxton22-Sapphire II
    22-Sapphire II
    April 4, 2024

    If I interpret the pictures correctly, then this is what you are targeting. I have enclosed a Creo 9 model using surface modeling and multibody get this geometry as seen below. This is to demonstrate a modeling approach that is feasible.

     

    tbraxton_0-1712248517128.png

    tbraxton_1-1712248570205.png

     

     

    A
    AIRMAN_DILLARD12-AmethystAuthor
    12-Amethyst
    April 16, 2024

    tbraxton,

     

    thank you for the sample model.  i could not get the sweep i started with to work, so i attempted your sample which is better.  however, i cannot get passed the solidify step.  what is the mkr2??  i do not know what you did at this point.  when i get to the shell feature, i can select sweep 1, but i cannot select offset 2.

     

    i also don't know what you used the other 2 lines for, if those are relevant.

     

    i'd appreciate your help again.

    tbraxton
    22-Sapphire II
    tbraxton22-Sapphire II
    22-Sapphire II
    April 16, 2024

    MKR2 is a comment line in the model tree, you can ignore it as it has no bearing on the other features.

     

    The other two lines are there as they can be used as trajectories for a variable section sweep to create the enclosed larger duct walls in a single sweep feature. I did not do this for clarity so you can see the intersection more clearly. You can ignore them in the context of the intersection.

     

    I used multibody to quickly create the geometry of the intersecting solids such that they can be used to create the part models for the large duct and the intersecting part.  Below MKR 2 you will see that the features involve two bodies as shown in the model tree design items. The grey and yellow geometry shown are two separate bodies in the model. The expanded tree shows which feature are used to create each body.

     

    tbraxton_0-1713232506658.png

     

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