Frustrated (New-ish) User

[Xwheelguy]

I've searched all over the net trying to find EXACTLY how to change Generative Drafting dimension arrow sizes. I find suggestions, but none work.

I have v5 (R18 SP6) in admin mode and can edit and/or save my standards. I'm using an open type arrow head and every stinking setting with open arrow type that I change has absolutely NO EFFECT on the selected dimension arrow once I hit Apply or OK. Do I have to restart CATIA for this to take effect? Can it even be done???

I've read that it can and I've also read that it cannot be done. Which is right and if it can be done, HOW? I'm about to scream because I'm working on a small area of detail and the arrows are just impossible to work with, to the point that I cannot see my geometry.

I've tried with and without views on the drawing (this is just something in 2D, no associated 3D/model) and no luck. I'm about to just give up and fire up NX.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[Xwheelguy]

Also, how can I set the default font for dimensions?

Thanks to anyone that can offer some help!

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[Xwheelguy]

I finally figured it out...none of the settings take effect until you create a new drawing after you save the standard. So I guess you are unable to change arrow parameters on the fly or go back and edit them in the current drawing.

Wow, what a pain.

Thanks to those that took the time to read.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[jackk]

thanks for sharing your solution.

 

[Xwheelguy]

This thread was helpful in finding the exact area of the XML file to modify for the open arrow size:

http://www.eng-tips.com/viewthread.cfm?qid=127251

From past experience with NX (changed defaults aren't applied until next time you start NX), I figured that v5 might be similar, so I eventually tried creating a new drawing and that did the trick. After that, I edited the Standard via Options -> Standards while running v5 rather than editing the XML file in Wordpad. The lack of anything changing when I pressed Apply was really throwing me for a loop.

I wonder what the workflow is for editing settings for existing dimensions WITHOUT creating a new drawing? Anyone care to discuss or offer any tips?

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[DBezaire]

Tim,
There is a method in the madness of V5, when ever and where ever you access the drawing you will be using the standards it was started with. I am pretty sure you can not change standards mid drawing (Ansi --> Iso) but you can use the search function to select all dimensions and change them to what you would like.

Are you setup for everybody to pull the same standard file?

Regards,
Derek

 

[PeterGuy]

You can update the standard of a drawing (i think it is in the page set up). But you cannot change ISO std to ISO Std. You would need to go ISO to (ANSI or JIS) to ISO as CATIA does not check the contents of a standard it only looks to see if it is a different one, if it is the same it does not bother changing it.

 

[Xwheelguy]

It wasn't the standards or how they were set up to use. It was just finding the correct setting in the standard and figuring out that it cannot be changed and applied on the fly (mid-drawing, as you put it).

I've used Autocad, SolidWorks, Solid Edge 2D, Microcadam, NX and I-deas. This is the first time I've ran into a drafting module that worked like this in regards to dimension arrows and other settings like it.

A little surprising, but I'll learn to deal with it.

Tim Flater
Senior Designer

 

[itsmyjob]

you should be able to update standard mid-drawing as PeterGuy said.

start with std A, then change your mind about dimension arrow, create std B, update drawing from std A to std B.

Eric N.
indocti discant et ament meminisse periti ​

 

[PeterGuy]

If std B was based on std A you would have to switch to std C before switching to std B, otherwise it would not bother making the change.
(where std C was not the same base std as A or B. The standards still have some hard coded portion that makes ISO, ANSI, JIS standards different, and it is this difference that is checked when updating and not the content of the standard (this certainly was the case, I have not checked recently))

 

[Hrishiis]

nkwheelhuy, PeterGuy and all

On a partially related topic, I was just wondering if the CATSettings files that are updated every time we close a Catia session has anything to do with saving standards (Is there a separate file that is created?).

Or is it just the settings (positions of icons/the Catia session 'Frame' as a profile) that these files save. The files I think are:

'FrameConfig.CATSettings' and
'FrameGeneral.CATSettings'.

Please throw some light.

Rishi Mandyam
Automotive Design Engineer
Catia V5 R12 - latest
Chelmsford, UK

 

[DBezaire]

Rishi,
Catia settings are saved every time you exit and you are correct with positions of icons.

Regards,
Derek

 

[itsmyjob]

just confirming what DBezaire said, I will simply add that the drafting standard is not in the CATSettings but inside the CATDrawing or on a folder with other standard for reference.

Eric N.
indocti discant et ament meminisse periti ​

 

[TheTodd]

If you'd like to know the reasoning behind everything, I think I can explain.

It's all because of CATIA V4. With V4 standards were not saved as a part of the .model file. For the .model file to know what text size, font, etc to display, it had to reference the .prj files. With V5 now, drawing standards ARE saved into the .CATDrawing files. That CATDrawing remembers the standards for wherever you send it. I think it was Dassaults way of making the drawing file more robust and people wouldn't have to worry about sending so many files. But as a result the only way to make the OPEN file read the new standard is to UPDATE the OPEN file's standard by going to File>Page Setup (then follow what PeterGuy and others mentioned).

So this is why when you opened a new file, it read the edited standard, i.e. updated arrow (you might also consider renaming the edited standard file ex. ISO.xml becomes ISO_new.xml). Once you then save that file, it will save that new standard into the .CATDrawing file and if you make changes again, you will have to update it again.

I hope that helps with the understanding of this.

Todd

 

[Xwheelguy]

Seems I inadvertently started the Lazarus topic, because this doesn't seem to want to die a quick death.

Basically, after creating a drawing, you can change standards via File -> Page Setup and that is what I wasn't doing correctly (well, not doing at all to be honest). I was just modifying my standard and that won't cut the mustard in v5.

I've since figured out what I was doing wrong and have gotten the dimension arrows to a size of my liking and just created multiple standards for different arrow sizes. Thanks for all who helped. I greatly appreciate it!

Tim Flater
Senior Designer

 

[djblik]

Question for "TheTodd,
I remember in V4 we had to have seperate standard files for FORD and CHRYSLER etc. Is that still the case with V5, since they carry the standards they were created with?

 

[TheTodd]

If Chrysler or Ford (or any of your customers) use their own set of drafting standards, yeah, most likely you'll have their set of standards in your V5 standards folder so that you can create new drawings in their standard. I don't know if that answers your question. Give me some more details if it doesn't.

Todd

 

[djblik]

Todd,
We have a FORD catia and a CHRYSLER catia, they are both at the same levels but if we are going to work on a FORD job we start up the FORD catia. I am just wondering if we need to do that any more or if we could just have one catia to open up. We had an IT guy here that took care of all this stuff for us but they decided we didn't need him any more and so for the last 3 or so years we have just been limping along.

 

[TheTodd]

Just out of a hunch. I'm betting that those two were set up in order for you to have 2 environments. Right click on your icons for the two of them and if they have different Targets. If so, they are probably also pointing to 2 different sets of options, or CATSettings. CATSettings are different than Drafting Standards, they control all of the CATIA workbenches and 3D settings. All of these can be controlled too, the admin of the environment can lock down settings. So there may be a chance you need to keep the two because they may be different evironments. If they are not different, and only the drafting standards need controlled, then yes, you can go to one.

I STRONGLY recommend that you have someone that knows what they are doing if you are seriously going to consider dropping one. My recommendation, I wouldn't change the way you have it. In my opinion it's much better to have the two. There is more control and less room for mistake. Also, if FORD goes to a different release or service pack then CHRYSLER, you're going to have data transfer issues.

Hope that helps

Todd

 

[djblik]

Ok, thanks Todd. This was all very helpful