IDEAS Assembly command: Configurations Is there such in V5?

[begnor]

When using IDEAS, in Master Assembly there is a command called Configurations, which allows you to show manipulated representations of your assembly(or product).Configurations do not permanently modify the design position of the data, only to show the different positions temporarily. These are stored within the assembly model, and can be used at any time, to show different states of the assembly, like a seat moved forward or rearward. They could also be used to create an animation, by ordering the configurations into a sequence. Config's could also be used on a drawing, i.e. to show an exploded assembly, or an open and closed state. Can V5 do this? My employer has chosen to save disk space and not load the help documentation.

 

[jec3300]

In Catia they are called "scenes" I am not sure on the animation part.

 

[solid7]

Generally, what you are referring to can be done in 1 of 2 ways:

A) by using the Kinematics Workbench
B) using the "animated constraints"

Kinematics is a better application to use, but animating your sketcher constraints works well, for some uses. (especially single part models)


---
Professional and reliable CAD design engineering services - Specializing in Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[begnor]

can someone gimme a quick rundown on the use of scenes?

 

[solid7]

Scenes are used to capture a part in a particular state, without modifying the design configuration. (hence the name, "scene") One of the main uses of scenes, is for exploded view.

Quite simply, you enter the scene mode, manipulate the geometry, and take a snap shot. It is frozen in that state, unless manually updated within the scene, itself.





---
Professional and reliable CAD design engineering services - Specializing in Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[catiajim]

Tell your employer to install the help documentation!!!!!! It's invaluable! Disk space is cheap, and the documentation only takes up a gig or two. If they are really concerned about disk space, have them install it to a network drive, and let everyone share it.

Worst case, they can install the PDF Documentation. This only takes 1 CD (~600MB). It doesn't include the sample CATIA files, but it will help.

 

[steveg501]

Yes very nice tool in I-deas but not available in Catia V5 R16
Most companies won't fork out the extra £12k plus training for the Kim package.
I would also be interested if any one has a solution or a substitute for this, Scenes just don't capture it like I-deas Configs.
One system I currently use, but is not as easy, quick or forgiving as the I-deas config system is;

Create a sketch to show driving geometry, show the sketch in the assembly.
Say I have a diff, Cv joint, drive shaft and hub arrangement.
The Geometry sketch shows the limits of the drive shaft, Metal to metal, GVW, rebound and roll conditions.
Constrain the geometry so it slides that is the drive shaft slides in and out of the cv joint as the hub moves up and down constrained to either a spline path or plane.
Creat two constrain sets for say roll and one for metal to metal – rebound conditions.
Just constrain the hub axle to the various conditions then to achieve the different config positions you activate or deactivate the relevant constraints.
I also had to create lateral plane conditions in each set but it managed to manipulate the assembly into the different configs by the activation / deactivation technique.

This technique allows you to work on the assembly while within the config without changing the setup.

If anyone has a better technique please let me know.
Cheers steve501 (sgeraci@prodrive.com)