Mirror of a part in an assembly with open bodies 2

[lordrailie]

Hi,

I'm trying to m,ake a mirror of a part inside an assembly, that just contains a few open bodies with surfaces, which I want to mirrro, but when I try to do an assembly mirror, the new mirrored part is empty, it just works with solids in main partbodies!!! Does anyone know how to go around this?

Thanx

 

[solid7]

First off - be specific - what version of Catia V5 are you using?

Secondly, my advice, is as follows:

1) in the assembly, Insert -> New Part -> "No" for origin of assembly

2) Create nothing in the new part. Call it "plane"

3) Use whichever plane you want for the mirror plane, or rotate it and transform it into position.

4) Use the Insert -> Symmetry function.

5) follow the directions as given.

Using the new part called "plane" you can modify the relative location of the planes, (and, hence, the symmetry distance) without having them tied to any other geometry, unless you contstrain them to something. (suggested - make an offset, preferrably) It makes changes REALLY simple.

I duplicated this in V5R15 before posting.

 

[lordrailie]

I'm using r14 sp4


What I wanted is to make the simmetry of a part inside an assembly that contained surfacic elements (more than 1) as we are doing preliminar designs (of yachts) using surfaces mainly, as they give us more flexibility. The problem is that when doing assembly simmetry it just takes the solid in the main partbody.

I found yesterday a way around that, that is using visual simmetry inside the freestyle workbench. but was not easy to find...


Thanx anyway

 

[solid7]

I did an entire hull and subframe in surfaces, with no problem. I've not even heard of "visual simmetry" (sic)

As a matter of fact, I've just verified my findings with a surface model. I had no problems, whatsoever.

Just as a matter of curiosity - what is your level of experience and proficiency with V5, and with assembly modeling in particular?

 

[lordrailie]

The insert simmetry you make is an assembly simmetry or a gsd simmetry???

For me it would be perfect to make an assembly simmetry, as most of the spaces are simmetrycal, and every space contain several parts or subassemblies. the main problem when you get to that is that, you have to create or
1- the visual simmetry (from the generic tools toolbar i FS)

2- new part that contain mirrored geometry from the rest of parts. Inconvinients, they dont have the same material applied so for visualization you have to redo it, its not the same structure, and is tedious.

3- assembly simmetry, as I said befoer, it just takes the main body, and the sirfeace you select as external view, wich is only on (no use)

I am using V5 for more than a year now, and i?m doing the whole assembly of the yachts we are doing, form surface design and styling, to detail design of parts, Structural analysis and rendering. Still not not good in knowledge. Assembly modelling is not a problem at all, but it took time to structure the whole precess, as I came from Microstation (in which i was modelling the whole yachts, including systems, furniture etc in 3d)

But everyday i realize more that this piece of soft is the way to go, even having little problems from time to time.

 

[solid7]

Well, you asked me about making a symmetry in the context of assembly, right? I didn't assume that I should, therefore, give you a GSD symmetry.

It appears to me, based on what you are saying, that you are inexperienced in Assembly modeling. Forgive me if I'm wrong - I'm not trying to insult you. I'm just saying that your comments and questions sound like those that come from V5 assembly newbies. Learning Assembly workbench is quite a task, even for some seasoned CAD users. Additionally, your spelling indicates that you are not working in a native english environment, and that you are possibly free translating the commands. That is also NOT helpful.

I'd like to help you more - if you're willing to post an email address, or point me to someplace where I can get in touch with you personally, I'll be happy to assist you further.

 

[lordrailie]

I asked mirroring a part in an assembly (product) with openbodies

I have no problem at all making a Mirror of a part containing a solid inside the main partbody

Before asking in the forum I tried what you said. I don't use the part you call plane, as I have a part with geometrical references where I can take the plane from. But doing the process you say, the result I obtain is a symmetrical part that just contains the main part boby, which for me is useless (at this stage), and at all the tests I made, the assembly mirror did not worked with surfaces.

In the catia documentation says:

"If the product to duplicate includes a part composed of several bodies, only the part body of this part is taken into account by the Symmetry command."

Also says

"Parts Including Surfacic Elements
If you need to perform a symmetry on a part including surfacic elements, the application creates the corresponding symmetry provided that an external view of these elements has been previously specified.
Conversely, if these elements have not been specified as such, the symmetry cannot be performed.

For more about the External View command, please refer to the Generative Shape Design User's Guide.

In the Assembly Symmetry Wizard dialog box, the External View or Part Body options inform you about the result you will obtain. For example, if the Part Body option is checked, the Symmetry command will affect the Part Body, not surfacic elements."

"You can define the Generative Shape Design feature that is to be seen when working with another application, such as Generative Structural Analysis for example.


To do this, while in the Generative Shape Design workbench:

Choose the Tools -> External View... menu item
The External View dialog box is displayed.
Select the element belonging to a Geometrical Set that should always been seen as the current element when working with an external application.
Click OK in the dialog box.

The selected element will be the visible element in other applications, even if other elements are created later in the .CATPart document, chronologically speaking.

To check whether an external view element has already been specified, choose the Tools -> External View... menu item again. The dialog box will display the name of the currently selected element. This also allows you to change elements through the selection of another element. Note that you cannot deselect an external view element and that only one element can be selected at the same time."



The part I want to mirror contains several openbodies with a large amount of surfaces.

Bear in mind that what I am doing now is not detail design but conceptual design and for that purpose I find it more helpful to create a product with various parts which contain only surfaces. A simple example is having a cabin in port side of a yacht, which is all contained in one part with 10 or more open bodies, and I want to have a mirror of that cabin (part) in the starboard side.

Thanx

And sorry for the spelling

 

[solid7]

Quite simply, you need to just stick with doing a copy and paste, to create a new instance of the part, and then manipulate the geometry with the compass, until you achieve a suitable position to apply a constraint.

Now that I've seen the part,(that you sent to me) I'm convinced that this is the only way to do what you are asking.

I'm really not sure why a symmetry is even an option in Assembbly.

 

[solid7]

I'm sorry, it's late at night and I'm grumpy...

Assembly symmetry is an OK option... Just not sure how the comment slipped into my writing. Can't edit on this forum.

Hmm.

 

[lordrailie]

The way I found that works, is to make a visual simmetry inside freestyle workbench, which creates a new part inside the assembly mirror of the first one.

 

[solid7]

Did it do an opposite part, or just copy the original in a 180 degree rotation?

 

[lordrailie]

A 180 degree rotation has nothing to do with a SIMMETRY!!!!

 

[solid7]

Yes, I know that. I was asking not about the method, but what the END RESULT turned out to be. Does it look like a TRUE SYMMETRY, or does it look like your ROTATED it 180 degrees? (the difference between an array, or a left hand / right hand part)

You seem angry that I would ask such a thing. I'm not sure if you know this, but it's always a good thing to ask what someone else is doing when you can't see over their shoulder. Believe it or not, sometimes people ask questions that either don't make sense, or they ask in the wrong way.

Not nice to talk like that to people who go out of their way to help you...

 

[JuhaEdag]

Hi Solid.
Freestyle Visual symmetry gives you a true symmetry (not a rotation). It doesn't create any geometry it's purely visual and can be used by surfacers to check curvature e.g in a hood only represented by half of the geometry or simply for a presentation picture.
I understand lordrailie's problem with the assembly symmetry though. We use a lot of surface geometry in BIW. An example would be a door outer panel made comletely with surfacic elements. When I want to show it in the assembly without duplicating the geometry it would be useful to use the assembly symmetry. It would also give you the advantage that when you change the left door the right door would automatically change (a common problem you forget to update the other side because it's symmetrical).

 

[JuhaEdag]

Hi Lordrailie.

To solve your problem actually just clearify Solids earlier messages.
Create a new Product, Insert a new part (right click the product insert new component).
Now right click the new product and insert existing component (which is your part with surfaces, solids etc.).
Now select assembly symmetry with your new product active.
Select the plane from the empty new part (probably the XZ plane depends on application of course).
Select the part you inserted (the one with the surfacic elements.)
and Whoops! there is your symmetry!!
Follow exactly the steps and don't worry it confused me as well it's not really that user friendly e.g why you have to create an empty part just for your symmetry plane?
I had the same problem earlier when I was working in electrical trying to flatten a harness. You must select the plane from the new part!!

 

[lordrailie]

Hi JuhaEdag

I've tried that just now in various different manners, but had no success. Whenever I use the assembly simmetry, I just get the main part body (even if I have 10 bodies, I just get the first) and no surfaces from the open bodies!

Thanx

 

[JuhaEdag]

I know it is confusing but it's typical Catia.
You must follow the exact order!!!
If you try inserting the new part (with your mirror plane) after you inserted your component with partbodies and open bodies you will only get the first part body.
It sounds stupid but that's the way it is.
1. Create new Product
2. Insert new part (under the new Product)
3. Insert one or more of your existing components
4. Make the assembly symmetry.
This is the only order that works for me. But it works with several parts (if you insert them together) and the parts can contain several part bodies and open bodies.
It only works in this order why I don't know it's a bit strange perhaps solid7 can explain why!
Is it a bug? or perhaps it has to do with the part identifier
UUID(?).
We're running v5r12sp5 HD2+ license on WinXP sp1.

 

[lordrailie]

I have v5r14 sp4, and following you steps, 1 by 1, I only get the first partbody!

weird?

 

[JuhaEdag]

Hi Lord railie.
Here is another tip to hopefully solve your problem.
Activate cachemode and make sure the part you want to symmetry is in visualization mode before you attempt to symmetry.
I noticed that the part will not symmetry if it is in design mode but after the symmetry you can activate the part no problem. Strange indeed!
Hope it works in r14 as well.

 

[lordrailie]

I'll give it a try on monday... and tell u the result

cheers