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.

 

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.

 

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

 

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

 

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

 

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

 

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

 

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

 

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