TEXT to sktch?! Help!!! 2

[hchen1228]

hi,

how can we put the text in sktch. seems no way(except copy from *.dwg) in catia v5r11!
this is a very very important feature and we can find this feature in almost any cad program (pro/e, solidworks, etc.), but why not in catia v5r11(or whatever in any version)???

any body can tell?

 

[CATMANDO2]

I found this somewhere on the net...- Create a new CATDrawing. Select a simple font and appropriate size. Select the Text Icon and a location near the origin of the default view. Save the CATDrawing for later reference. Save the same file as a .dxf. (This creates line segments.) Open the .dxf and select the lines, Copy (Ctrl+C). Create a plane on the part that you want to emboss. Create an offset plane or surface to define the pocket bottom of the embossing text. Select the Sketcher Icon and the Sketch Plane. Paste the .dxf lines (check orientation) and translate them into position. (This can be tedious.) Return to the file saved in Step 4, if the text requires mirroring. Exit Sketcher and select the Pocket Icon. Use Up to Surface for the second limit and select the other plane/surface.
If this is not what you want perhaps you need to change modules to "Functional Tolerancing and Annotation", you can type in anything, anywhere. However, this will not give you text within a sketch. This is the module you use for Model Based Definition.

 

[hchen1228]

Hi,

thank you for your help.

because i used work on designed cast parts and request put cut/extrude compeny logo and part number in surface of each part. i currently use this techique, but first of all, it is so inconvient, 2nd i failed in multiple characters.


in pro/e's "area offset" function is so easy to use.

i still do not understatnd why catia v5r11 is missing such an important feature.

I appreciate your help

 

[johnny5ng]

Hi, Catmando2

I created some texts in Drawing with "inches" set up and saved as .dxf file. When I open the .dxf file, the text become very small. Look like the text was compressed into "metric".
Then, I made my text 25.4 bigger in Drawing and saved as .dxf file, When I open it, the text become right size.

My Question is: how can I can save my .dxf file in "inches" format?

Johnny
jng@contouraerospace.com

 

[catiajim]

Tools, Options, Compatiblity, DXF tab. Note: If you are going to re-import it to CATIA, set it to mm, as CATIA's base unit is metric.

 

[johnny5ng]

Catiajim

Thank you, it work fine...... but
In catdrawing, I chose Aerial o.4 and save as .dxf
When I open it, the text become hollow, and too close together.....
Actually, I want to have a stick like letter that I can drive my center drill for engraving. How can I do that to get the "stick like" letter??

Johnny

 

[puck]

Try the Monospace font.

 

[johnny5ng]

Thank you Puck.

I tried Monospace 821BT ( true type ) and Monospace 821, both are not working, I also tried another fonts, I got the similar results......
I am F-king tired of Catia engraving, I would rather use MasterCam to finish that simple work.
U know, I am not trying to do the advance engraving like the CatiaPartner "

http://www.type3.com".

What I need to do is to script the Part no. on the fixture.......CatiaV5 makes it so hard.

Johnny

 

[catiajim]

We ended up writing a script to do this for us.

Have you tried using one of the V4, Stroke-Based fonts such as SSS1?

 

[johnny5ng]

Thank you, Catiajim

I know V4 can do that, but V5 missing that area.
OR
May be V5 has that function and no one find out.......
OR
Catia keep it in OPTIONAL feature for more $$, who know.

Anyway, I use MasterCam to finish those "HARD TASK".

 

[catiajim]

In V5 there should be several "V4" fonts available (unless your System Admin has locked them out). They are the SSS1 thru SSS4 (as well as a few others). These are the V4, Stroke-Based fonts that should work. The other fonts are all postscript, and are bit-mapped fonts that have trouble translating well into 3-D.

 

[johnny5ng]

Finally this problem is solved. Thank you all of u guys

http://www.coe.org/forums/attachments/How_to_create_TEXT_for_engraving.doc

Johnny

 

[tiasimo]

WHY USING SSS2 AND SSS4 AND NOT ANY OTHER FONT?

 

[catiajim]

Because these fonts are Stroke-Based, and will translate to 3-D as lines and vectors. The PostScript fonts are all bitmapped fonts, and there is no equivalent geometric object in a CATPart document.

Actually, any Stroke-Based font should work (in other words, the letters are all made up of lines and curves, not area-fills).