Auto-create a model to fill the assembly

[pellet8]

I created an assembly which forms irregular inner surface. You can imagine it is like the inside of a room with all kinds of furnatures installed in place. To model the fluid flow in the empty spaceof this "room", I need to create a part that fills all the space in it, in other words, a part whose surfaces matchall the surfaces of the furniture inside as well as the walls. Does proe provide a automatic tool to create such a part? If not, what will be the easiest way to created it? Thanks for your advices.

 

[pellet8]

Anyone knows? Please.Thanks.

 

[Miko]

I really dont know but You maybe need to create assembly in Pro/Moulding module. Or try to create your assembly like one part from surfacs. Than try to use solidify feature. [:s]
Edited by: Miko

 

[Jacoolo]

that is really not nice situation


well, unfortunately there is no tool that will perform that or I do not know if it exist


the ways I proceed in such situation depends on things I want to achive.


Some times it is very fast and easy to collect all inner surfaces to Publish Geom and put it in another file


sometimes I make a Shrinkwrap which gives me a shape without inner geometry and than make some cut out or so


sometimes You can just collect sketches of inner geom and put them in new file and use them for desired geometry


You can also merge parts in assembly with Edit>components operations>merge

 

[Moroso]

Did you try Shrinkwrap

 

[dojo]

If there is not to much geometry in it, i would throw the fluid part in you assembly, and then copy the contact surfaces with copy geometry. Unfortunally you have to create a new copy geom for every single part. Go to the part merge the quilts and solidify. Ive not come across this problem alot except for some fluid washer tank which is ofcourse simple to do...


Another option would be to create as mentioned above create a swrinkwrap as a merged solid of your assembly and then (external) copy geom the inner surfaces.


Regards,


Nick

 

[Zaki]

Hi Pellet


Just create a blank part then copy all inner surfaces of room and solidify it, then perform cutout feature to remove all parts from this geometry.

 

[Zaki]

Hi Pellet


just create a blank part and save it, then assemble it into assy as u like, after that activate it by rmb in model tree, set selection filter to geometry and select one inner surface of room, then copy n paste, in paste options u can select all inner surfaces of room, then set selection filter to quilt and select copied quilt>>solidify. After that u can do cut out operation by activating the assy. may this will help u!!!

 

[james.lynch]

Zaki's way is a parametric way.. works well ..


you can also use insert/advanced/cut out from other model ( I think that's where it is off the top of my head (or maybe insert/shared data/cutout from other model)


As morso said.. Shrink wrap is a great way to do it..I saw a presentation by John Randazzo (spelling?) at PTC user a fewyears ago where he used teh fill holes option of shrink wrap to create a solid of the outer most surfaces.. then used the best settings without fill holes (9 - not 10, 10 causes crashes) create the true geometry, and cutone from the other.. worked really wellfor CFD...


James

 

[Isair]

I assume that you must create "fluid" part because of analysis, and fluid part must have density, and other psychical properties (analysis in cfdesing?).
So I think that easiest way is to create new assembly, put in it, assembly with "room", create fluid part and put it in new assembly. For fluid part just create either tube or rectangle, or shape it like outer surface of your room (just use constrains of room in this new assembly). Now create component cut; Edit > Component Operations > Cut Out > select room asm, and fluid part.
When you finish, fluid part will have shape of space in room.