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TEXT ON CURVED SURFACE-PAPERSPACE PRINTIN

nitan

New member
I need to put extruded type on a curved surface. Not sure how to do it, on a flat one is easy. Here is the model if you have an answer.


2006-04-08_032438_22mm_petcock-stem.zip


Also, when I print a drawing, all of the lines and type on the titlesheet (that was from the format template) as well as some dimensions, and the profile linesprint very fat lines and get unreadable. But the dimensions from the layout viewports come out very thin, whereas the dimensions that I add come out fat.


I think this is a difference between paperspace and modelspace, but I could be wrong. How can I make all of the lines and type thin lines so they are readable?


I have Pro-E Wildfire.


Thanks for any assistance.
 
To get text on your surface, from the top toolbar, select EDIT, then Project. On the dashboard, select references. Click the down arrow and change "Project chains" to "Project sketch". When the sketcher button appears, open sketcher. For the sketch plane, make a datum that is offset .600from the "FRONT" datum. This places the sketch .05 above the surface that you want to project to. Select "TOP" as your reference plane. When in sketcher, on the top toolbar, selectsketch, then Text. Sketch your text and dimension it so that it is over the surface you want to project to, and select "Done". Now back on the dashboard, highlight "No items" in the "surfaces box". Pick the surface that you want to project to. Highlight "No items" in the "Direction Reference" box. Pickdatum "FRONT", and flip the arrow until it points towards the surface you want the text to be on. Done.
 
To fix your print problem, there are config.prooptions, pen1_line_weight, pen2_line_weight,...., pen8_line_weight. Start with all pens set at "1" or "2". Then adjust the weight to make which colors you want to be fatter. "1 = thinest". "16 = Fattest".
Edited by: appinmi
 
u can also use draft offset command, byset selection filterto geometry, then edit>>offset, then selectView attachment 2098this, u can use a previously made sketch or define a new sketch. U can see a topic previously posted here by name of text on 3d surface.
 
Thank you for the replies. I did get text on the part, but I want to extrude it into the part 0.015" and remove, engraved letters.
 
If you use ProNC to create the CNC code, Create a cosmetic groove using the same method as you did with the datum curve. When in ProNC, create an "engraving" sequence. Within the parameters of the sequence, there is "groove depth".


If you just want the engraving to appear on the part, create a surface that is offset .015 from the surface you want the engraving on. Use your datum curve but change the text font to a "3D" font, (closed letters). Now extrude the cut using the edges from the datum curve with the depth set to "to selected", and select the offset surface.
 
I want to show engraved letters on the part, just not understanding how to cut it into the part on the curved surface.
 
Thanks for your help. I was able to extrude to the surface that I had created under the stock surface. It wasn't a projection, but it worked.
 

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