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MSa1-Visitor
1-Visitor
June 17, 2014
Question

Filled text

  • June 17, 2014
  • 3 replies
  • 15698 views

Hello

I´m modeling electrical enclosures and labels for them with Creo Parametric 2.0. I´m trying to make them by modeling a label base where necessary texts are cut extruded. Then I make a drawing and print it to the aluminum foil. Obviously by using this "technique" only outlines of the text is printed and the gaps between the text outlines are so small that the result is not looking very nice.

The question:

Is there way to put a filled text into a planar surface of a part? I know that I could add a text in to the drawing but then the text wouldn´t follow the model and copy pasting the model to the next project wouldn´t work.

3 replies

KenFarley
KenFarley21-Topaz II
21-Topaz II
June 17, 2014

The method I use to put text, logos, or any other graphics onto the surface(s) of a part is the "Cosmetic Groove", which is under the "Engineering" (I don't know why) tab. You pick the surface(s) you want your geometry to be on, then sketch the stuff you want projected onto the surface. Planar surfaces are the easiest, but I've used this a lot on all sorts of curved surfaces. The reason I use "Cosmetic Groove", generally, is because I can use these types of features to engrave the parts using the manufacturing module.

A recent improvement to Creo is the ability to use a parameter for the text in the sketch, which makes it really easy to have family table parts that have unique text such as part numbers, etc.

Hopefully this is what you were seeking. I don't know if a lot of attention is paid to this type of feature in the general Creo userbase, but I use it a lot.

M
MSa1-VisitorAuthor
1-Visitor
June 17, 2014

Thanks for the answer but I can get only outlined text with this method. Is there way to fill the text?

D
dschenken1-Visitor
1-Visitor
June 17, 2014

See http://communities.ptc.com/message/244054

    Patriot_1776
    Patriot_177622-Sapphire II
    22-Sapphire II
    June 17, 2014

    Cosmetics are pretty worthless IMPO. I use sketched datum curves exclusively for this type of thing, making labels, doing silkscreens, and such. You can make the curve have hatching (you have to go back into it and add the option - really stupid), and then at the dwg level you just make the hatch spacing so small it prints solid. Bing able to use parameters in sketch mode (sometimes driven by relations and/or other parameters - model_name, and Windchill revision etc.) is awesome.

    Good luck!

    KenFarley
    KenFarley21-Topaz II
    21-Topaz II
    June 18, 2014

    But can you use datum curves to make a feature that has a complex logo and included identification text, projected onto a contoured surface, and then use it for engraving? I've always used the cosmetic groove stuff to do this, so I can mark contoured surfaces with a ball endmill. It's been a while since I tried any other method because this one has not let me down.

    Patriot_1776
    Patriot_177622-Sapphire II
    22-Sapphire II
    June 18, 2014

    You can project or wrap a datum curve. Complex logo's are going to be tough in any feature if you're trying to have a bunch of entities in a sketch. You might have to make several sketches. I made these labels in Pro/E, and made some curved ones as well, I just can't find the images. You can also float a surface .002 or so off a solid surface for silkscreening. 8408-012_2006-07-10_01.JPG8200-187_CLOSED_SILKSCREEN-01.jpg

      M
      MSa1-VisitorAuthor
      1-Visitor
      June 19, 2014

      Thanks all for the answers.

      Below is shown the printed drawing in to the aluminum foil. Drawing is made from a part where sketch is extruded to the label base. Geometry line thickness is too wide but not enough to fill all of the center areas. Result is blurry and messy.

      Extruded-sketch.JPG

      When I make an annotation note in drawing, the result would be accurate enough for me (see another photo), but then the texts will not follow the model and the placement handling is not so flexible as it is in part level when feature is sketched. Also drawing notes are not shown in assembly.

      Drawing-note.JPG

      I copy paste these labels all the time and modify them so easy handling speed is needed. Maybe Creo is not the right platform to do these things but I have been happy that I can modify the panel cut outs and these labels at the same time and see the result in assembly.

      Propably filling the text is not even a solution. I would need accurate printable text somehow in to the part´s surface.

      T
      TomD.inPDX17-Peridot
      17-Peridot
      June 19, 2014

      I am glad you provided the additional information.

      This is a separate problem.

      The problem is that the text gets assigned a pen thickness that is added to the outline of the text.

      This can be solved with pen tables.

      So pick a method of making the text solid... filled geometry or extruded solids.

      When you print the drawing, use a pen table to manage thickness of the printing (very thin!)

      This works for your line art as well. Make it to the size you want and set the pen thickness to .001" for instance.

      You probably need to print using drawing views with "shaded" views. I have also created shaded views under hidden line views to make the outlines crisper. Setting the environment to black and white, you will get very good output.

      Are you printing directly to a printer or to a PDF output? I am not as familiar with direct printing outputs but I know I can get there with PDF.

      If you want, you can attach the file to these messages by using the advanced editor (upper right of the reply dialog). I can show you what can be done with PDF without too much effort.

      T
      TomD.inPDX17-Peridot
      17-Peridot
      June 19, 2014

      And you may be right, this is certainly not the tool to make "camera ready art" but it can be made to work for the specific instance you are looking for.

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