CREO 10 SWEPT BLEND ON A CURVED SURFACE

[AIRMAN_DILLARD]

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.

[tbraxton]

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.

[AIRMAN_DILLARD]

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]

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.

[AIRMAN_DILLARD]

I CAN GO BACK AND TRY THE SWEEP AS A SOLID THEN SHELL.  I'VE TAKEN ALL THE CREO CLASSES, AND HAVE BEEN USING CREO FOR SEVERAL MONTHS, BUT I AM STILL SEMI-SKILLED IN USAGE.  I AM NOT SURE WHAT YOU'RE REFERENCING FOR "PROXIMAL AND DISTAL FACE SURFACES".  I DO NOT RECALL THIS IN THE CLASSES.  WOULD YOU PLEASE EXPAND ON THIS.  THE PLANAR SKETCH IS AT A SLIGHT ANGLE/PITCH COMPARED TO THE LARGE BODY, SO WHEN THE SWEEP COMPLETES IT CREATES A SMALLER ARC ON ONE END OF THE SWEEP

[tbraxton]

I am referring to the proximal and distal ends of the duct. These are arbitrary, and not unique to Creo. For fluid handling designs the proximal face would traditionally be the inlet.

[AIRMAN_DILLARD]

THANK YOU FOR YOUR HELP, I WILL PLAY WITH IT AND SEE

[tbraxton]

For fluid handling components I would typically use an inside out design approach. Since the wetted area of fluid geometry is usually critical to function, I would design a fluid master model to represent the fluid volumes using curves and surfaces. I then use this as a guide to build solid geometry to take constrain the fluid and deal with any boundary conditions and other design constraints.

This is an example of a fluid master for an injection molded manifold. The fluid paths are the purple and the orange are valve bores that control fluid logic among the circuits. This also expedites CFD simulation work on the fluid domain during the design phase.

[achirila]

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]

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.

[AIRMAN_DILLARD]

THANK YOU FOR ALL YOUR HELP.  THIS GIVES ME AN ALTERNATIVE FOR ANOTHER MODIFICATION.  LET ME EXPLAIN, SORRY FOR NOT INCLUDING THIS (IF I FORGOT), THE BASE BODY IS AN EXTRUDED CUBE, THEN SHELLED.  I HAD TROUBLE THINKING ABOUT THE BEST WAY TO GET THE OVERALL SHAPE I WANTED AND APPROACH FOR THE BOX BODY, SO I EXTRUDED A CUBE, THEN CUT THE EXTERIOR TOP SHAPE AND SIDE CUTOUT, EDGE ROUNDS...THEN SHELL.  THIS I BELIEVE (NOW) IS NOT THE BEST DESIGN APPROACH FOR WHAT I AM AFTER FOR FINISHED PRODUCT...AFTER THE FACT WITH ALL THE FITS I'VE HAD.  AS YOU DID, I SHOULD'VE USED SURFACES TO CREATE THE BOX, THEN THICKEN...I PROBABLY WOULDN'T HAVE THE PROBLEMS THAT I'VE HAD.  BUT...IT'S WHAT I HAVE RIGHT NOW, I WILL ATTEMPT SURFACES FOR A MODIFICATION WHEN AVAILABLE 🙂

[MartinHanak]

Hi,

please do not write in CAPITAL LETTERS.

[AIRMAN_DILLARD]

I USE UPPER CASE BECAUSE OF MY VISION, LOWER CASE BECOMES JUMBLED TOGETHER

[AIRMAN_DILLARD]

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]

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.

[AIRMAN_DILLARD]

Again, thank you for your time and help.  For whatever reason, I just can't get this to work.  I get all the way to the last step "solidify" and it won't regenerate (I can't get it to remove the material from the "surface" that was generated for the sweep from the opening, flip the arrow and it will remove the outer perimeter surface but not from the opening).  I've double checked every option and step in your sample.  I will give it one more attempt.  I don't want to burn out my welcome, but if I can't get it, are you open to review my file?

[tbraxton]

I am happy to review a file, but I do not have Creo 10 installed yet. Creo 9 or Creo 7 I can open the file but not 10.

When you are completing the last solidify make sure that you have the yellow body selected as the active body, so the material is removed from the desired body.