Patterning fasteners

[fighterpilot]

Scenario: Plate in assy w/ 5 holes. Holes are not part of a pattern in the plate. Have fastener, would like to place one fastener in a hole with surface contact and coincidence constraint. Now, how do I get the other 4 holes populated w/o placing each individually? I'd like to pick the surface, define it as common to all fasteners, and then select the other 4 axis and have them populate.

V5R14SP1 on Windoze 2K

Thanks for the assistance.

 

[Configurator]

Power copy?

 

[fighterpilot]

From the help files:

Select the Insert ->Advanced Replication Tools -> PowerCopy Creation menu item.
The PowerCopy Definition dialog box is displayed.

These picks do not exist. Something seems to be amiss.

 

[Configurator]

You need the PKT licence.

 

[fighterpilot]

I give up. I've selected the PKT license and still don't see the picks outlined above.

I could go into a raging diatribe about Catia but I won't. I was at the COE last week and determined that Dassault suite was about 5-6 years behind PTC's offerings. Guess I'll just step back into time...

No flames please..

 

[Configurator]

^^ Depends on what you want to do. If you are doing loft-heavy hybrid design or advanced surfacing, V5 is ahead of everyone else.

 

[KooKoo]

Try creating a "dummy" part with a User Pattern then in the assembly use the Reuse Pattern. If you don't select to create a link to the "dummy" part you can delete it after.

 

[catiajim]

What fighterpilot is trying to do is in Assembly Design, so a PowerCopy won't work. He needs to create a Product Template, which does indeed require the PKT License.

Another option is a VB Script. I wrote one a few weeks ago that allows a user to select a surface and multi-select a series of points to place the fasteners. It also requires a secondary orientation, even though you don't normally care about this for screws and bolts. Basically, this script takes the location of each point, creates three normal vectors based on the surface and secondary orientation curve, and places the instance at that location/orientation. It doesn't create any constraints, but that should be fairly simple to do as well.

 

[fighterpilot]

Power Copy?, PKT license?, VBScript?, dummy part?

All I want to do is repeat the placement of a component multiple times.

For example in Pro/Engineer: Component/Adv Utils/Repeat. Done.

It shouldn't be that hard to do. Hence my comment about stepping back in time.

 

[Configurator]

"What fighterpilot is trying to do is in Assembly Design, so a PowerCopy won't work."

Whoops. </stupid>

"Power Copy?, PKT license?, For example in Pro/Engineer: Component/Adv Utils/Repeat. Done.

It shouldn't be that hard to do. Hence my comment about stepping back in time."

Does Pro/E not have licence configurations? You get every option all the time? That's kinda cool...

 

[fighterpilot]

Yes, You get nearly everything you need, except things like Mechanica and NC which is a separate license. PTC used to do what Dassault is doing, nickel and dime you for every package, but got away from it after user complaints. What Dassault is doing is simply making it difficult for the user and the administrator. Especially when you have to restart after selecting a license.

 

[Configurator]

^^ I think the difference between Pro/E and CATIA is scope. CATIA has WAY more functionality, and it's unrealistic to ask every user to pay for every function. How often, for example, do average mechnical designers need circuit-board design?

It's hard to predict what functions any given user will need, but they tried to do so with the different licence configurations (e.g. HD2 is meant for the common design engineer working to lofted surfaces).

I suppose Dassault does offer a (pretty much) all in one package for most designers. It's called SolidWorks.

 

[catiajim]

And actually, if you had placed your Holes in your Plate using a User Patter, instanciating your parts is a simple matter of using the "Re-Use Pattern" button. The problem that you are having is that you stated in your first post that the holes were not originally created as a Pattern.

If your plate is flat, and all of the holes are parallel, placing the holes and the parts is a trivial operation. In our case, however, it is not that simple. Our holes are located normal to a complex surface. This forces us to use a script.

One of the beauties of having a tool like VBScript is that it allows us to extend CATIA in ways that DS didn't expect.

 

[Akesson]

I totally agree with fighterpilot that the kind of functionality that he asks for (repeat insertion of parts) is one of some functions in the Assembly Workbench that you miss if you come from the ProE world.

ProE is superior Catia V5 in many ways (especially the drawing creations) but what I like about Catia is that it lets you create your models in many different ways and the Knowledge ware is great. I prefer the Catia user interface even if ProE Wildfire 2.0 is much better than ProE ever have been before.

I always hear from Catia users that Catia is much better when it comes to surfaces. What I understand is that the Catia surfaces have a higher accuracy than ProE surfaces. When it comes to creation of the surfaces I think ProE ISDX surfaces is really great, not that many Catia users that have tried this.

The perfect 3D-CAD-program isn't made yet... :c)

/Akesson

 

[catiajim]

What good does it do, however, to create surfaces more easily if they are not accurate? Perhaps in some industrie this is OK, but in the Aerospace and Automotive industries, we must have very accurate surfaces, albiet accurate means different things to each of us.

 

[Akesson]

Catiajim,

You are probably right about that you need Catia in the Aerospace and Automotive industries but in other areas like consumer electronics and many other plastic industries I think ProE is accurate enough. It could never be a disadvantage that it's easy to create the surface....

Always great discussions when it comes to Catia V5 vs. ProE
I have the pleasure to use them both on a daily basis. Things that are great in one program could be bad in the other and vice verse.

/Akesson

 

[fighterpilot]

Akesson,

Can I use you as a resource to make the connection between Pro/E and Catia? I'm struggling right w/ the simplest of things because my brain is thinking Pro/E functions. 11 years of Pro/E is going to be hard to flush.

I didn't want to start a Catia/ProE war, I was just looking for a way to quickly assemble a bunch of fasteners. My parts were imported from another CAD system so I didn't have the luxury of reusing part patterns.

Thanks...

 

[Configurator]

"I always hear from Catia users that Catia is much better when it comes to surfaces. What I understand is that the Catia surfaces have a higher accuracy than ProE surfaces. When it comes to creation of the surfaces I think ProE ISDX surfaces is really great, not that many Catia users that have tried this."

It's not just the surfaces themselves where V5 shines. It's designing with and to surfaces (hybrid design). That functionality is unmatched by any other CAD system, and Aero/Auto is DSS's target demograph (for V5).

IMO, it is also superior to the other CAD systems in terms of its parametricity. I've never worked with a CAD system that offers better collaborative design.

Like anything, once you learn it it's easy, but also like anything, before you get to know it it's hard - especially if you come at it expecting functionality exactly like some other system you've used.

 

[Akesson]

Fighterpilot,

I suggest that you try the functions "Fast Multi Instantiation" (Ctrl D) and "Define Multi Instantiation" (Ctrl E). These commands in the Assy Workbench is the closest to "Repeat" in ProE you can get (They let you insert the part that you click on). The difference is that you have to constrain them. To make the creation of constraints easier/faster when for an example instantiating fasteners I can recommend to use the "Stack Mode" function in the "Constraint Creation" Toolbar.

Use it like this:
- Select "Stack-Mode" from the "Constraint Creation" toolbar
- Doubble-click on the "Coincidence Constrain" button.
- Select the mating-surface that all the bolts should be attached to.
- Select the mating-surface of the first bolt.
- Dialog opens, click ok
- Select the mating-surface of the second bolt.
- .....

Hope this gave you some help.
I'll try to give more help if you need.
If you find any functionallity like ProE "Spinal Bend" in Catia please let me know.

/Akesson

 

[fighterpilot]

Configurator,

I always thought Pro/E had very good parametric design capabilities. One function I really liked was I could have an assembly open in the main window and then close that window and then call up a part (of that assy) into the main window. When you closed an item window in Pro/E, it would not remove it from memory. Everything stayed in memory for a quick retrieve. You could really use this to your advantage sometimes. I've caught myself attempting to do the same in Catia and usually end up losing my changes because I close a window w/o saving the item first.