Various V5 Questions

[thixoguy]

Hi All,

I have a few V5 questions I was hoping a few of you might help me out with.

1. What is/are "apply dress up" "remove dress up", and what are the advantages to using it/them?

2. How do you create/extract "non associative" curves or surfaces?

3. Is there anyway to create N.P.T. type threads? Also
is there a quicker way to create imperial threads? I remember seeing somewhere that you could import an excel spread sheet with the proper tap drill sizes and thread pitches. I wouldn't mind trying to create one on my own if someone could explain the procedure or set me on the right path. The thread creation capabilities of Catia really leave a lot to be desired.

4. Finally, is there some sort of "settings" you need to set when you import, for example, a socket head capscrew into a product file? I find that if I import a screw in the "Mold Tooling Design" package I get the screw that I have selected,and it also creates the necessary boolean removes on the appropriate components. However, if I simply want to import a screw in the assembly (not in the Mold Tool design packege) and want to constrain it manually, it seems that no matter which screw I select in the standard Catia catologues, I always get the same size screw. I am using version 15 and am wondering if others have the same problem?


Thanks to all who take the time to respond, thixoguy

 

[solid7]

1. Right click -> Propterties. "Dress up" is when you apply centerlines, axes, hidden lines, 3D wireframe, etc. The advantages/disadvantages are obvious.

2. Use the "datum element" toggle before selecting the extract function. Click once to use it one time, double-click to keep it "running". (find more on the subject in the help docs)

3. Create your own spreadsheet or tab delimited document for defining the threads. Simply locate the standard file for the existing threads, pay attention to the format, and make yours accordingly. Then, save it in the same folder. As for the thread capabilities - there is not much value in graphical representations (pretty pictures) of threads. (you can dimension to the thread callouts in Catia, though)

4. I believe that you need to break links to the catalog after you resolve the part. (so as not to revert back to the template) Someone else should elaborate on this, because that's the way I do it, and it may not necessarily be correct.

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[jackk]

just to add a little to Solid7's answers:

2. Use the DATUM ELEMENT before extracting, or right-click and ISOLATE the element to drop the associativity after it's been extracted

3. Many people have asked the same question previously, and several people have provided the files required for inch (UNC and UNF) threads. I don't recall seeing NPT threads. Suggest you search this forum and other forums for "INCH THREADS" (I wouldn't be surprised to find them on Solid7's website)

 

[solid7]

2. Use the DATUM ELEMENT before extracting, or right-click and ISOLATE the element to drop the associativity after it's been extracted

Unless I'm mistaken, or don't have my glasses on, ISOLATE is only an available function for points and lines.

The other workaround for isolated geometry, is to COPY and PASTE AS RESULT.

Suggest you search this forum and other forums for "INCH THREADS" (I wouldn't be surprised to find them on Solid7's website)

I definitely have inch threads. Follow my sig file to the CATBlog.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[jackk]

Ooops! I misspoke about isolating extracted curves and surfaces - sorry!

(thanks for correcting me, Solid7. Apparently your glasses work much better than my memory! Maybe I was using the V4 side of my brain?)

 

[solid7]

No problem jackk... It happens.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[thixoguy]

solid7,

Thanks for the info..I have downloaded the inch text files from your site( thank you also to DBezaire for creating and sharing files)

My next question is where do I put these files so that I can use them in Catia? I can't seem to locate where my existing (metric)files are located. Can you direct me?

Also,I have tried to use these files during thread creation in the hole feature( I have "added" them) But when I access them under the "thread description" I only see zero,s. Any suggestions on what I am doing wrong?

Thank you in advance,thixoguy

 

[solid7]

C:\Program Files\Dassault Systemes\B1X\intel_a\reffiles\standard (replace B1X with your version number - i.e., B14, B15, etc)

If that's not the exact location, search your computer for "reffiles".

My suggestion for what you are doing wrong is that you are using the "add" function. Place those files in the standard. Also, make sure that you are using tab-delimited text, and not space delimited. You can verify this by opening the document in MS Word, and turning on formatting. It should show Tab characters between information columns.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[thixoguy]

solid7,

I have placed the files into the proper folder but I am still getting zero's under the thread description tab. So I would like to investigate the " tab-delimited" text you speak of but uhh.... what exactly is tab delimited text?
I have opened the thread files in MS word but I don't really understand what I'm supposed to be looking for?
Any further suggestions are greatly appreciated.

Thanks, thixoguy

 

[DBezaire]

Thixoguy - open the file in a text editor - notepad. You need a tab inbetween the text (a spacebar hit is consider text). To evaluate the file, place the cursor on the line item, use the left/right arrow cursor to advance through lettering. If your cursor jumps several spots - you found a tab.

NPT Settings:
Make a NPT.txt file in the above directory that Solid7 referenced.
NominalDiam(in) Pitch(in) MinorDiam(in) G
0.4190 1/27 0.3450 1/8 NPT
0.5180 1/18 0.4380 1/4 NPT
0.6580 1/18 0.5795 3/8 NPT
0.7980 1/14 0.7090 1/2 NPT
1.0020 1/14 0.9370 3/4 NPT
1.2360 1/11 1.1560 1 NPT
1.6390 1/11 1.5000 1 1/2 NPT
2.5000 1/11 2.1880 2 NPT

Large spaces are tabs. I can email files if you like.
The pitch is not required for my use - they are not verified.
Regards,
Derek

 

[thixoguy]

DBezaire,

I couldn't quite get your file(which I downloaded from solid7's site) to work so I made a copy of the original catia metric thread file and simply editted it to suit my needs- it worked. In any case, I am grateful for the help both you and solid7 have provided. I also plan to incorporate the NPT data which you have so kindly taken the time to provide.

thixoguy