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CATIA V5 best practices
5

CATIA V5 best practices

CATIA V5 best practices

(OP)
hi!!!

   R there any best modeling practices to be used with Catia V5...any tips?

Thanks,
Jay

RE: CATIA V5 best practices

2
here's a few tips that are open to discussion:

1. always fully constrain sketches (sketches should be green or yellow - never white)

2. always do a sketch analysis before you exit a sketch

3. limit the use of boolean operations

4. when working with assemblies (products), always use SAVE MANAGEMENT (if not using a PDM)

5. always publish elements that will be linked to child parts, and only make external references to published elements

RE: CATIA V5 best practices

Hi,

See also FAQ on this forum

Regards
Fernando

RE: CATIA V5 best practices

Hi,

When you create a Hole on a non-planar face of a solid :

Create a point on the surface, the axis of the Hole and a plane normal to the axis passing thru the point.

Then Pre-select the point and the plane when you create the Hole.

In other words: when you create a Hole on a surface, never clic on the surface!!!

Eric N.

catiav5@softhome.net

RE: CATIA V5 best practices

Hi,

To create a new exemplar of a CATPart based on an existing one it is very important to use “File/ New From” command and not “Save As” command! “New From” creates a new exemplar of an existing one and prevents problems in the product structure.

Never use planar surfaces (its better to use planes) for sketch support because its easier for changing the sketch- support if you want to make some modifications.

For better performances in creation of a catpart, features like fillet, chamfer, draft, shell a.s.o. should be used whenyou finish the catpart, so these features will be at the endof the specification tree.

Keep sketch as simple as possible to make modifications easily. Don’t create geometry which can be created as features, i.e. fillets, chamfers, holes. Don’t use mirror function in Sketcher, use it in Part Design.
Auxiliary elements have to be created as construction elements because otherwise the
sketch doesn’t work correctly

Use Auto Search command to select all elements of a sketch profile easily. Select only one element of the profile and run Auto Search with the right mouse button .

Use Auto Constraint command to constraint the whole sketch easily.

Regards
Fernando

RE: CATIA V5 best practices

jay24:

-Keep your tree well organized and take the time to rename the elements to something that makes sense. It will make it easy on anyone else that uses your file.

-Give a lot of thought to applying relationships and constraints. They can cause you, or whoever has to update/modify your file, a lot of grief if not carefully created.

Terry

RE: CATIA V5 best practices

Ferdo...

What's wrong with using Mirror inside a sketch?

I do it all the time. A simple example is two parallel lines that are centered about an axis. Sketch one line and the axis, then mirror the second line. Constrain the total distance between the two lines. Works great!

...Jack

RE: CATIA V5 best practices

I think there is nothing wrong with using the mirror inside the sketch also I don't think there is anything wrong with using radii in a sketch(instead of fillets) it's very easy to change the radii in a sketch and a lot of times using fillets outside the sketch makes the geometry very heavy and complex.
It all depends on the case if I have a simple extrusion like a gasket why would I use fillets???
However in more complex designs it might be more useful designing to hard corners and fillet afterwards.
Think before you design, rules don't work all the time (but it can give you a good direction).
I also heard a lot of times that converting from Catia v4 to Catia v5 is soooo difficult, thats bullshit if you were a good designer in v4 able to use solids it should not be that difficult.
The hardest thing to overcome as a v4 user was the links and doing packaging because we were not used to the assembly structures like they have had in Unigraphics for a long time.

RE: CATIA V5 best practices

I agree with JuhaEdag.

I can see no logic to putting fillets/chamfers outside the sketch.  Sounds like carry over methodology from V4 to me.

We design a lot of machinings with complex revolutions and it is far easier to see all the chamfers/fillets in one sketch.

RE: CATIA V5 best practices

Actually, I think the fillets issue has more to do with the Drafting Representation.  Fillets can be displayed in many different ways, but corners in a sketch cannot.  They can only be displayed with or without the tangent edges.

RE: CATIA V5 best practices

Actually, the beauty of sketches is that you can change it so if your'e not happy with it take the bloody corners off!
Like I said think before you design it all depends on application. The Gasket was maybe a bad example ( because I never done one my self) but I would imagine it is cut by some kind of stamping tool (what is the draft used for then?).
I have worked in BIW, Interior design, I-P design, A-class surfacing, Seatings and recently Electrical design and I still think if you can incorporate your fillets in the sketch you will have one less of operation to worry about.
However like I said before it all depends on application if you have deep draws you would of course design to hard corners then draft your surfaces (solid walls) and fillet.
There is many applications though where you can sketch with corners (i.e you have two sketches and you run a surface or a solid to create your shape between the sketches, First sketch is much larger than the second this will give you draft naturally, why in the world would you want to add draft when you already have draft by the shape? it would be easier to change the shape of one of the sketches to allow more draft).
It all depends on application don't misunderstand me I use shapes without fillets all the time especially in moulded plastic parts but if I can incorporate it into my sketch I'm happy it makes updating easier and in the end I will have enough fillets to fight with for sure (no xtra needed).
    

RE: CATIA V5 best practices

Drafting as in 2-D Dimensioned drawing. Unfortunately, we are still stuck with these.

RE: CATIA V5 best practices

I'm truly Sorry I thought we're talking about making the parts from 3-d data. Sorry about my ignorance but last time I did a drawing was in Italy 2000 and It was so boring doing all those mega drawings (to make managment happy), fortunately v5 seems to be aiming to get rid of most of it!

RE: CATIA V5 best practices

Whatever works best for the situation. If I am doing a 2D shape that is being extruded or cut out with a laser or even simple shears then go ahead and put in the fillets(gaskets and such). If I am doing something a little more complex then hold off on putting them in the sketch. Alot of times the fillets need to be deactivated to ship to an analysis group. The order that they are applied can be critical as well. Never fillet then draft. If you do the fillet is no longer a true radius. Things like that.

RE: CATIA V5 best practices

What is Catia Publish?
Why is it important to make external references (for child parts) only to published data?

RE: CATIA V5 best practices

DOES ANYONE KNOWS HOW TO EDIT THE TITLE BLOCK AND BILL OF MATERIALS WITHOUT USING A MACRO, ANS STILL KEEP THE LINKS TO THE COMPONETS AS PART NO., DESCRIPTIONS AND SO ON.

THANKS.

RE: CATIA V5 best practices

Arvindsathe....

Publish provides several advantages over non-published links, but the biggest is when you do changes to the parent part.  If the parent part is replaced or renamed or if the published geometry is replaced, the links will be maintained and the child parts will remain in-sync. Non-published references must be replaced manually.

RE: CATIA V5 best practices

Hey MGONZALEZ41

You have to Attributes links:

1-During the text edition, right-click on the background and select Attribute link
2-Activate the 3D document and select the component witch you want to read the value from.
3-Back in the 2D, select the appropriate attribute/property from the available list.

Good luck

SaP

RE: CATIA V5 best practices

Keep sketches simple. V5 is FEATURE BASED. I can handle complex sketches, but it will bog down the system. I often have nothing more than a line in a sketch.

This should be obvious, but I see it a lot, so here goes: Don't use windows to re-name, copy or move files. You're begging to screw up UUIDs (and thus links) if you do so.

Work with cache if you have large assemblies.

Someone mentioned booleans above. Avoid them when they aren't necessary (ie: do a pocket instead of a remove, etc.).

I disagree with ferdo on this one: don't use auto-constraints. It's best to explicitly define everything yourself.


The main thing is to be aware that in parametric modeling systems, everything is kept track of.

RE: CATIA V5 best practices


Avoid links between parts in an assembly. Use skeleton parts if you want to use linked parameters and geometry. Links like this makes Catia slow. Important when you work with large assemblies.

Constrain your sketch to the planes and not to H and V axis (the big yellow ones).

Always use a positioning part (a part containing plans etc as reference when positioning other parts) in your assemblies. Add a "Fix" constrain to it. This makes eveything fixed to the "absolute" coordinate system of the assembly.

As said before, only link published geometry/parameters.

If you make the links from a skeleton and a part when they are in the same context the pointing feature of the link is shown in the name of the link.

Only sketch on planes (not planes that are created with any reference to the solid or surface) not on a face or a surface. This will make your model more stable if you would like to make changes to it.


RE: CATIA V5 best practices

here's another best practice to add to the list:

Do not make sketches over complex with alot of constraints in order to drive a single feature. It is better to break the design down into many features that are based on simple sketches.

RE: CATIA V5 best practices

Why try to limit Boolean opertions?  Surly using boolean features stabilises the model when modifying.

RE: CATIA V5 best practices

Darrude....

"limiting the use of Booleans" means use solid features instead of booleans whenever possible.

Yes - booleans have a purpose and should be used. But they shouldn't be used like they were in V4 for every operation.

RE: CATIA V5 best practices

With regard to Booleans, I invite methodology advise on the following:
I work in aircraft. The parts, such as front and rear spar, for example, are common to contour on the top and bottom flanges. Most of the stiffeners are orthogonal to the web; some may be canted. The webs (pocket floors) have pad-ups, and the flanges and stiffeners have steps that generally don't line-up with the pad-up steps in the floor. Using the features within the main body to create these complex machined pockets very often results in an inability to fillet afterwards and split lines where these features come together to form the steps in the flanges and stiffeners. I have found that creating separate part-bodies that are pocket features that have been split to the contours, canted planes and step locations, filleted, and then 'assembled' into the main part body, which removes the material as a pocket, works well and results in a more simple tree...??  
What are some other good methods for these complex parts?

RE: CATIA V5 best practices

Hi,

Since May 2004 (when it was my initial post), I've changed a lot of my initial opinions about best practice in v5.

Best practice? That one which is required by your client (and a lot of some others already posted here).

Regards
Fernando

RE: CATIA V5 best practices

l3ob,
Yes, in your case booleans are necessary for the performance and stability of your part.

I think that the initial admonitions against the use of booleans have more to do with using features, as jackk points out.  In V4, we used to subtract a cylinder to create a hole.  We used to subtract a cuboid or prism to create a simple pocket.  In V5 it is preferable to use Hole or Pocket for these simple shapes.  Obviously, in more complex situations are definitely necessary.  

The real point is to use whichever tools are easiest and most stable to accomplish the job.  Don't go out of your way to avoid booleans. But don't go out of your way to create them either.

RE: CATIA V5 best practices

hi

When I use boolean operation, for example assembly the body is stay on the place where was before. Not goes with the assemlby to another body.

RE: CATIA V5 best practices


catiajim,

In your response to l3ob you mention the "stability" of part models.  Can you elaborate on what you mean by model stability?  How can the use of booleans affect stability?

RE: CATIA V5 best practices

Sometimes fillets work better on external corners than they do on internal corners.  In this case, you would create a "negative" Body for the pocket, fillet it, and then assemble or subtract that from the main body.

Other times you may find in a very large solid that your performance will be faster if you can group features together (like in V4 with the "horizontal tree").  

Still other times, it might be easier to create a bunch of bodies and then assemble them to the main body. Then if you change one of them, you don't have to update the entire tree, just the branch that you changed (and anything below in the main branch).  Take for example a part with 100 holes.  If you create the Pad, then create each hole one at a time (pretend for the moment that a Pattern doesn't work).  You end up with a "vertical" tree that has no boolean operations.  Then, if you change one hole near the top of the tree, the entire part has to update. This can take a very long time.  Or what if you need to delete the first hole?  If you had taken the common approach of selecting the functional surface of the solid for each hole, your entire solid will blow up - since each hole below relies on the functional surface of the hole above, which was deleted.  In this case, creating a bunch of negative bodies outside of the primary body will leave each of the holes independant of the others.  Another solution here, of course, is to extract the face of the solid first and tie each hole to that extracted face.

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