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Raised text

I need to add raised text and a raised logo to a surface. The surface is not flat, it curves in all directions. I created a curve in the shape of the logo (for simplicity, lets say that it is a triangle) as a sketched curve on a datum plane in front of the surface. then I projected the logo curves onto the surface. I tried to "OFFSET" the projected curve, to get the raised thickness. It works if set to "along surface", but when set to "normal to the surface" (what I want), it only offsets one of the curve lines. Because the surface is not planer, I can't use "FILL" to change the curve into a surface and then use "THICKNESS". It is worse trying to project text because when it asks for the curves to project, it only allows one line of a letter at a time (letter "T" has 8 lines around) and even so, it says that the ends of the lines are not connected so it won't make a surface from the projected curves. I have also tried STYLE with no better results. I have read the rediculous HELP files until my head swims but can't find anything of any use. Is Proe WF3 capable of doing this? Any help is appreciated. Peter.

Reply to
Peter
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Wow. This would take all of 10 seconds in SolidWorks.

Here is what I would do... might not be the best way Offset the surface a distance (height of text) Extrude the sketch of the text (oulines of letters) then trim with the offset and original surfaces.

Reply to
Aggrevated

I agree that this is a simple operation in lots of other CAD progs, but it is rather difficult for me in Proe. I suspect that there is an easy way to do it but I can't find it. I was not able to offset the surface (grayed out) but I can thicken it to the height of the logo. I extruded the logo sketch onto the original surface but I can't trim the extrusion (also greyed out). Even if it worked, the text should be a different thickness than the logo which is on the same surface. Also I need to use thicken to make the surface thicker in the other direction (a different thickness again). Peter

Reply to
Peter

First, create a new surface as copy of your part´s adjacent surfaces (the ones to carry the logo). Then another using "offset" to this. AFAIK ProE does not create offset surfaces from solid surfaces at once.

A logo solid extruded to the part can be trimmed using offset surfaces, as long as the solid is completely inside the surface boundaries.

Or: extrude the entire logo into a surface (closed loop letters) then merge with an offset surface, and "use quilt" to solidify. Again, the surface boundaries have to be completely inside the solid.

Dunno what these steps are called in FiledWire, I´m still on 2001. I know ProE since V12 - so I guess there´s not much difference inside.

Walther

Reply to
Walther Mathieu

Walther, I followed your suggestions but I can't get the solid extrusion to trim (greyed out). TRIM is only available when a SURFACE is selected, not a SOLID. I tried to make the extrusion into a SURFACE but the result isn't what I wanted. Thanks for your help Peter

Reply to
Peter

Copy the surfaces you want the text on, project the text through these new surfaces as a surface trim, and thicken.

Reply to
John.R.Wade

Don't use trim. Use "thicken" and select the "cut" option.

Reply to
Aggrevated

Don´t mix surfaces and solids in ProE - entirely different approaches.

Can´t "trim" a solid. As I told you, the name for it may have changed, earlier on it was "feature", "create", "cut", "use quilt" for a solid to be trimmed using an offset surface or "feature", "create", "solid", "use quilt" fore a more sophisticated one (i. e. the complete logo made up from an offset surface).

You will then enjoy to select all tangential edges of each logo letter for neutral curves ... "feature","create","tweak","draft","neutral curve" back in 2001.

Sorry if this is not of much help in WF eventually.

Walther

Reply to
Walther Mathieu

Something went wrong with the posts and replies and David Janes sent an email to offer suggestions. Below is a summary of the emails between us.

Here's how I did what I think you're trying to do.

  • Select the solid surfaces; they'll turn salmon colored
  • Click 'Edit>Offset'
  • Get the Icon for 'Expand', not 'Standard Offset Feature'
  • Set the expand distance
  • Get the Options menu and click the Sketched Region radio button for the 'Expand Area'
  • Define your sketch
  • Make your side surface Normal to Surface (last radio button)

You don't even need to project the curves onto the surface and you should get raised text based on your sketch.

David Janes

Glad to see you got my solution and that it worked. Well, it's interesting that it works for everything BUT text. Maybe it's the kind of text you're using. For starters, I'm pretty sure this'll work only with vector geometry. Pro/e's fonts qualify, so does True Type and PostScript and so does anything in DXF. So, if I create a sketch with the Sketch Tool and pick the Text icon, I can make text from any of the PS/TT fonts. In the Offset tool, it may be necessary to use this sketch to create another where you reference the sketched text with Use Edge. So, it may be just a matter of finding a suitable font. But it will produce raised text this way.

David Janes

Hi David, as you said it does create raised text. I was trying to use the text directly and this doesn't work. I did as you suggested and by using EDGES it works a treat. One point of interest is, if the surface uses curves for its shape, the raised text may fail if any part of it crosses a curve.

Thanks again Peter

And thanks to all who replied. Much appreciated. Peter

Reply to
Peter

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