advantages to using Create Datum mode?

[jackk]

In a recent post, someone said they need to create geometry with CREATE DATUM activated. I read this to mean that their models are created with everything isolated and not associative. To me, that's wasting one of the biggest benefits of V5.

What are the advantages to using CATIA this way?

 

[PeterGuy]

Create datum does have some advantages, but you are entirely correct you are throwing away one of the major advantages of V5.

an example where create datum can be useful is:-
Following the repair of an imported model. i.e. you fix the model, but all the features you create are just adding to the data size so using create datum enables you to get the final surface and throw away all the preceeding data.

Some users use create datum and no keep mode to make V5 behave like older system for example V4.

 

[slcad]

I´m the one using datums a lot...

I don´t know about you guys, but I´ve had a lot of "great" experiences with complex parts where more people worked on the same file and the result was a complete mess... And being the last user to work on such files, I was not very happy about it...

Our company designs plastic-part molds. The parts come from our partners, most of the time not fully moldable, so we need to work on them a little bit and then build the 3D "split-line", actually the split-surface. Because the parts are very complex, we decided we use the old v4-style of splitting the core/cavity plates and sliders with "a skin". To have this done, we would practically kill ourseves by keeping everything associative...

I´m a fan of associativity myself... But from my experience, I found sometimes it doesn´t necessary help. I use a "hybrid" solution (my version of hybrid design ) where I join together associatively large non-associative surfaces ("skins"). I usually work associative until I reach the final result, than I "deassociate" it, for the sake of file handling.

The example from the other post (about the sketch) was one step in creating some help-surfaces for my "skins".

Finally, I think it´s a matter of personal preferrence and company policy, I won´t enter in any debate about it...

Regards,
Stely

 

[solid7]

NOTE: I've been trying to post this response for days. This site is always broken or acting up!

You don't really mean to say that you believe that ALL pieces of geometry in a model need to be parametrically associative, do you? That is, EVERY SINGLE PIECE OF GEOMETRY back to the model creation? (!!!)

Jackk - parametrics are great when you need them - but not everyone needs them - or at least not all the time.

Example:

I have a model that requires me to build a balanced rotational part with 4 blades. Because I don't trust Catia to solve the radii properly, (half will solve in + direction, and half will solve in - direction, and I can't control that) I create some extraction geometry to build some points for a variable fillet, and then revolve it. But I don't want to keep the extraction geometry. I only want the resulting points to control my fillet. So what do I do?

I use datum elements, of course.

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[solid7]

Although I think I understand what you are trying to say, Catia is much better than some programs in this particular area, in that it gives you the OPTION to select when to use parametrically linked geometry or not. If you think about this, you will begin to understand that it avoids having to use multiple or external models for reference (skeleton) geometry, or humongous models which complicate data management, yet add little value.

Datum elements is a blessing. Besides that, elements (not part features) allow you to redefine the data parametrically later, so you really don't lose anything. You can't do it with features - like extracted faces - but we can't have it all now, can we?

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Catia Design|Catia Design News|Catia V5 blog

 

[catiajim]

One suggestion to solve the ambiguity problem of CATIA not knowing or remembering which direction things go: Create 6 points in your seed model. One each at +/- 1000in along each direction. Name each one Positive_X, Negative_X, Positive_Y, Negative_Y, Poositive_Z, Negative_Z. Now, when you want a re-usable part and are having problems with direction, create an element each direction, join them (with Check Connexity turned OFF), and then perform a NEAR operation, selecting the appropriate point from above.

Yes, it adds a few more elements to your part, but it will vastly improve the stability of your templates. This method works realy well with PowerCopies and UDFs.