Is CATIA really this deficient?

[aardvarkdw]

So, I've been using CATIA for about 4 months now and I am getting competent with the tools I need to use. I was a little disappointed when I found some basic tools that I used daily in other software was not available in CATIA but I got past that and have found other ways to do what I want.

However, there are several glaring things that I just can't wrap my mind around. For instance, why is it that every other 3d modeler out there utilizes the origin planes and encourages the user to constrain to them as often as possible as they are the most stable features (being first in the tree and system defined)but CATIA seems to discourage this (every class I have taken has made a point of telling us to NEVER attach to the origin and instead to fix components or to dimension to the origin after the rest of the geometry has been built). The other glaring thing I found today is that CATIA's drafting module does not appear to have a tool for hole callouts...This floored me! Sure the push is to go toward using ASME Y14.41-2003 for MBD but you still have a need to create 2d drawings sometime. I can understand not having an ordinate or a stacked dimension option or not having chamfer callouts but hole callouts?!

Would someone please tell me if I am wrong and point me in the right direction if there is a way to generate a hole callout from the model. I would be most grateful.

Thanks.

David

 

[fighterpilot]

David,

Lemme guess, your "other" software was Pro/E?

Yes, you can use a hole callout in a drawing. In a drawing select Insert/Generation/Generate Dimensions.



--
Fighter Pilot
Manufacturing Engineer

 

[aardvarkdw]

No actually I used to use Autodesk Inventor and Solidworks.

But that is beside the point. I tried your suggestion and all I got was discrete dimensions for the diameters of my counterbored hole. What I would like is a hole callout per ASME Y14.5M-1994 which I believe most programs even 2d programs can now produce.

David

 

[fighterpilot]

Yea, you gotta use the Functional Tolerancing & Annotation Workbench to add the GD&T symbols. It's kinda confusing in V5. Pro/E for example would just let you add that info right to the driving dimensions. In V5, you can model one way and dimension another. I don't agree w/ it but that's what you can do.

Start/Mechanical Design/Functional Tolerancing & Annotation. This assumes of course you have the license for that workbench.

--
Fighter Pilot
Manufacturing Engineer

 

[m1mason]

your statement "CATIA seems to discourage" constraining to origin is not true. Whoever told that does not know what he's talking about. In fact, it is highly recommended. The only reason why I think they said that is because when you click on an element (ex. line) and select the origin right away, the software "glues" the geometry to the origin. It seems that it cannot be removed from there. Solution: select the break command and click on the origin. It will release the element.

That's why we avoid the origin initially. you create away from it, but then constrain back to it, since, like you said, it is the most stable reference.

http://mtm-cadtutorials.blogspot.com/

 

[catiajim]

The "CATIA seems to discourage" constraining to the origin part is a hold over from a long time back. Up until about R11 or R12, there was only one kind of sketch available, the "Sliding Sketch." In it the origin was forever fixed so if you were creating geometry that you wanted to change with the location/orientation of the geometry you were forced to NOT constrain to the origin.

When DS finally gave us the "Positioned Sketch" this is no longer a problem.

 

[fighterpilot]

catiajim is correct. Positioned sketch is much better. I use it all the time.

--
Fighter Pilot
Manufacturing Engineer

 

[aardvarkdw]

Thanks guys(gals?),

I hadn't looked too much into positioned sketches. It was one of those things that got mentioned in class but was never discussed afterward. I'll look at that. It is always frustrating to learn a new system after you are fully indoctrinated to another one but CATIA just seems to go out of it's way to make it difficult some times. Can anyone shed some light on where to find the option to change the default drawing annotation (dimensions, text, etc...) color? Everything comes in white for some reason and disappears into the background. I've looked through all the options but I cannot find the defaults for "graphics properties".

David

 

[brengine]

you can use a hole callout in a drawing. In a drawing select Insert/Generation/Generate Dimensions.

I believe this only will dimension the hole in a profile/side view, not in a plan view orientation were you're looking at an actual hole. "Other" CAD packages add the Hole Callout to the circular hole.

Ken

 

[brengine]

Attached is a Hole Callout example available from others. This is a native function that places a fully parametric Callout with the click of one button.

I am unfamiliar with "Start/Mechanical Design/Functional Tolerancing & Annotation". I will check into this myself as this type of Hole Callout is something I have been looking for with Catia as well.

Ken

 

[fighterpilot]

kchuck,

Hey that's a great hole callout. Pro/E would kick out the same thing all day every day w/o creating extra "tolerancing" callouts. You can attach all the information you need right to the model driving dimension which to me makes the most sense.

In Catia however, you model one way and then have to go back and place FT&A on your model after the fact. You cannot attach information right to a driving dimension. In fact, you could just violate the intent of your design and V5 wouldn't care. To me, that seems very backwards.

aardvarkdw,

Use Tools/Options and then work your way thru the tab and option to find all the various settings in V5.

--
Fighter Pilot
Manufacturing Engineer

 

[catiajim]

Can anyone shed some light on where to find the option to change the default drawing annotation (dimensions, text, etc...) color?

Yes, these are controlled in the Drafting Standards file. Here is a FAQ about doing this:

http://www.eng-tips.com/faqs.cfm?fid=1179

 

[m1mason]

In addition to using "Tools/Options" to change certain settings. you can manually override certain dimensions by right-click Properties or using the toolbars that relate to that.

but if you really want to change things permanently then you need to go to Tools>Standards. but there's a catch: you have to become an administrator in CATIA in order to change them. they will be grayed out if you're a regular user. Of course, That's a different discussion.

http://mtm-cadtutorials.blogspot.com/

 

[aardvarkdw]

So what you are basically saying is that my company has some how screwed me by making the default annotation color white and I have to get someone with administrator access to change this for me? All so I can create a stupid drawing. Wow, I think I need to cry in the corner for a while until I can come to grips with how ridiculous that is...

David

 

[m1mason]

David,

it is possible to become admin in CATIA V5 WITHOUT being admin in Windows. I created a video a while back that shows how to do it. it's alot of steps and quite complicated. but at the end you'll have full control over you environment.

http://mtm-cadtutorials.blogspot.com/2008/10/catia-v5-becoming-administrator.html

 

[weavedreamer]

Providing you are not on a network involving other users, and the files/directories you need to modify have the permissions set as required to enable editing?

While the background is default white in color, to set the text, etc. . . to white - someone must have had an idea of what they were doing?

The video looks technically correct, the graphics are difficult to read, or my reading glasses just keep needing . . . not going there . . .

 

[catiajim]

This is not a "problem" with CATIA! This is a requirement by many companies that insist that their drafting standards be consistent. This file controls many things like Dimensioning Style, Arrow Sizes, Available Fonts, etc. There are over 300 different attributes of your drawings that this file can control.

I'm not sure why someone at your end changed the color to White - the defaults are all Black on a White Background. You will need to get someone who has control over these files to fix them.