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How to Engrave Your CATIA V5 Model

One of the most commonly asked questions by trainees on one of our CATIA V5 Fundamentals courses is “How do I put engraving on my model?” By this, they usually mean adding text in the form of a pad (emboss) or pocket (deboss) to permanently identify the part. A simple alpha-numeric text string on a flat surface either raised or embedded by a millimetre or so will suffice.

CATIA V5 does not have this function built in as a directly available modelling feature.  I should mention that CATIA 3DEXPERIENCE does include an enhanced version of engraving directly from the sketcher workbench.

However, in CATIA V5 it is very simple to achieve:

1. Start by having the model you want to engrave open and ready to go, and create a sketch on the surface you want to engrave. (Make sure the model orientation comes up with the area where the text is going to be horizontal. If it doesn’t, use a positioned sketch rather than a sliding sketch to get the model orientation correct).                    

      

 

2. Now create a new document of type ‘Drawing’. I.e. Make a new drawing and use ‘ISO’ as the standard and the default ‘A0’ (landscape) as the paper definition.

3. Use the ‘Text’ function in the drawing workbench to create the text you require. I would suggest you position the text close to the drawing datum in the bottom left corner.

   

 

4. Once you have created the text, you can use the text properties toolbar at the top left to give the text the attributes you require. The default ‘Monospace821’ font works well. Set the text size to between 5mm and 10mm as required. Apply ‘Bold’ or ‘Italic’ etc. as needed. 

   

 

5. The next task is to save the drawing out as ‘DXF’. From the file drop down menu, select SaveAs and then select ‘DXF’ as the ‘Save as Type’.  Give the file a name and save it in an easily accessed folder. 

   

 

6. Next job is to load the DXF drawing into CATIA. File > Open then select the DXF you just created. (N.B. The reason for creating the DXF is that it is a convenient way to convert the ‘Truetype’ text into lines, arcs and profiles, etc.)

   

 

7. Once the DXF is loaded, zoom in on the text and either do a drag box or type (Ctrl+A) to select the text.

8. From the Edit menu select ‘copy’ or type CTRL+C.

9. Change window to the one with your model with the waiting (active) sketch.

10. From the Edit menu select ‘paste’ or type CTRL+V. The text should appear in the sketch. Whilst the text is still selected, move it into the correct place. 

    

 

11. Optional step. With the text still selected, scale it if required.

12. Exit the Sketcher.

13. Use the Pad (emboss) or Pocket (deboss) icon to create the solid geometry.

  

 


For more information or if you have any questions about CATIA V5/3DEXPERIENCE, please leave a comment below or email our helpdesk at support@intrinsys.com.