Comparing CATIA and Unigraphics commands 3

[LnTxn]

Anyone know of a link and/or chart comparing CATIA and Unigraphics commands?
I am a Unigraphics NX designer and trying to learn CATIA V5 and am having a difficult time learning the different commands.
Thank you in advance!



Stephen

 

[LowRoach]

Stephen I know your pain, I've spent the last 6 years using Ug from version 13 to nx2. I recently took this position using Catia v5. It took me about three months to discover all the catia/ug similarities. Altough I was able to start being productive right away with out any training. What are you major responsibilities in Catia? Part models, assemblies, or drawings? I can maybe write some tips up if I knew what areas your spending most of your time.

 

[LnTxn]

LowRoach
Primary and secondary structures.
Need to know solids, surfaces, assemblies.
Appreciate whatever you can do and I will do the same.
Going to write a word or excel document outlining the differences and when I do I'll pass it along.
Sure helps to know someone who feels the same way.
I have a few names of books if you want the names.
I'll post them later.

Thank You !




Stephen

 

[LowRoach]

This might seem simple, but I have to start somewhere.

The specification tree works like the model navigator.
In that tree you can use "Define in work object" the same as you use make current feature in UG. Lets say you have a part body with a pad, a hole and a chamfer. Now if you wanted to add an edge fillet before the chamfer you would define the hole as the work object.

All parts start with three datums, this is similar to the three fixed datums you could have ug put at x, y & z

Pad works like an extrude thats untied
Pocket works like an extrude thats subracted
Shaft works like a revolve thats united
Groove works like a revolve thats subtracted
If you wanted to duplicate an extrude or revolve thats intersected you would have to "insert, body" create your pad or shaft then use a boolean operation to achieve the intersect.

That brings me to a point I should hit on, UG is vary picky about having more than one solid in a part, it would restrict you if an action was going to create two solids. Sometimes the result would be un parametric solids. Catia deals with this different. You can insert multiple bodies and split things and still have two parametric bodies....

more to come.....

 

[LowRoach]

Just to be clear so far I'm only comparing the catia part design workbench to ug's application modeling.

I probably should have started with sketches.
First off catia sketches and UG's sketches are very much a like! If you are comfortable with sketches in UG then you will have no problem with catia sketches. Now if you didn't use sketcher much in UG you are going to be hurting in catia. Almost everything is built with a sketch, catia completely depends on them. There aren't even primitave solids to start with.

In catia skether you have constriants and constraints defined which are the same as dimensions and geometric constraints. These function pretty much the same. I think the biggest difference is catia doesn't have point on line, you use coincident by picking the line and point. Pretty simple.

There is a mirror function, it functions about the same. Also if you have construction geometrey that you set as reference in UG, you can do the same in catia, its called a construction element. Project 3D elements is a strong feature in catia sketches, its simalar to insert extracted edges in UG but a little simpler becuase you don't have to extract the edges before going in the sketch.

Also You can constrain to edge or lines outside the sketch in catia and ug about the same.

 

[LowRoach]

Next feature in catia is hole, guess what in ug its also called hole. Boths softwares allow straight holes, counter sunk, counter bored, flat or pointed bottoms,and tapered holes. Now I think a tapered hole in ug tapers from the hole start face, but catia tapers from the bottom face... don't hold me to that just be aware of it.

Catia has one additional hole type and its counter drilled, which is like a counter sunk hole sunk in, if that makes since.

The UG thru hole functionality is there in catia, but is accomplished by selecting, blind, up to next, up to plane or up to surface.

Hole intruduces another difference. Catia positions holes with a sketch where UG uses positional dimensions. In the hole dialog window the buttons labeled positional sketch. So thats not a big mystery. The first time you go into this positoning sketch you probably will be confused. It looks like every other sketch and it seems like its blank or empty. Not true, all it contains is one point and that point is all you care about. You're not in the to create the geometry or shape of the hole. You are just in there to locate that one point.... just like you did with positional dimensions. You can constrain it with constriants or constraints define (dimensions and geometric constraints). You can use edges, lines other sketches and etc.. to constrain to.

The hole is one place you can add threads in catia(its also a seperate command). I think its lacking some here, catia out of the box only comes with metric course and fine and thats it. And to make matters worse you can only make the simplified type. There is no way model threads in! Now i know the arguement here threads take a lot of time for computers to process and there not worth modeling, but at least you had the choice in UG.
Although I'm speaking about modeling threads have a big down fall in drafting too. In ug if you modeled simplified threads you could still show full threads on a drawing! Real looking threads, but not in catia just a simplified rep.

 

[LowRoach]

Well there is a start I will try to add more, but I need to do some actual work here today too. I hope this helps and I may have made a few mistakes so please comment or add.

 

[LowRoach]

oh yeah and before I forget the desk command is like the assembly navigator in ug. Its very fussy though and doesn't always like to replace or relink everypart. The "desk" will show you your assembly tree.

 

[ewh]

Steve,

It's good to see that your still in aerospace! Good luck with the transition to Catia. I have enough trouble going from NX2 to NX3!

Eric

 

[LnTxn]

LowRoach
Really appreciate the information !
Good to know there are people out there to assist and share information !
If you ever need help drop a line and thanks again !



Stephen

 

[UGperson]

When useing the pad, pocket or similar commands in catia, you can pick spacific lines like UG's curve, chain curve command by right mouse clicking the selection box. This is also how you redfine pad pocket or similar function. And dont forget

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