Embossed text in Part

[das_thunder]

I there!



I'm using PROE wildfire 3.0 and I need to recreate a design Part that resembles a car license plate.

As you can see the plates have embossed letters from both side (front (embossed) and back (grooved)) with a variable section sweep on the edge of the letters.

So I'd like to ask what's the best way to do this?

The great for me would be to do that in only one step (only with one feature) because I need to do a family table of several license plates!

Thanks

Edited by: das_thunder

 

[[-Skint-]]

Not going to be possible with only one feature. But you could get there with 4 or 5. If your happy using the standard text tool then you can create the text on your plate, then have one datum plane for the raisedtext and one for the sunken text. Depending on the level of detail you may have to create the sunken text slightly smaller so that you can raise it into the protruding text. Apply rounds etc and then when you want to create your family table all you would have to do is go back to the original text sketch and amend the text.


I am not too familier with the sheet metal part of pro-e, maybe someone will inform us that there is a simple " Stamping " feature that will do it all in one go

 

[tobbo]

Ibelive there is a feature that can do just that in sheetmetal....


Otherwise, i would probably suggest " offset whit draft feature" for the text . Then you dont have to do it in so many features.... (nothing wrong whit many featuers tho...)


maybe first do the "embossed" on one side , and then on the other side , use the offset feature again and use " offset edge" in the sketch..(and use the first sketch as referense) . then you will have a "wall thickness" automatically.


About the familytable..... when you do your sketched text , you can drive it whit a parameter, then you just have to change the parameter name and the model will update. (dont know if you can get it to work whit the " offset features" but if you use simple extrudes i belive you can..., otherwise you can probably drive it whit some dimensions instead , and get it to work that way

)


//Tobias



Edited by: tobbo

 

[SRINIVASANIYER1]

This is a case for sheet metal.
Create ONE punch and then create a family of punches...
for the different letters and different sizes.
Under sheet metal module...create "Form" to get what you
want.
If you want to do it in solid.... click on the 3D models
at the top of the page which will take you to
traceparts..where you will get embossed texts.
I hope this helps

 

[mstols]

Sheetmetal option will work.



or



It could be done with a solid part as well.
Follow these steps.

1) Make a solid block the size of plate. (Make the thickness a bit more than the required plate thickness. If the plate is 1mm, make it 2mm, I'll explain why later.)
2) Create a second solid extrude on the face with the text.(ex AAA)
3) Add the draft feature to text. (It is VERY important to use the seed and boundary option to select the surfaces to draft. This will allow you to change the text to anything else later and the features won't fail.)
3a) Steps for seed and boundary surface selection.
3b) Select the text feature. Then click on the top surface of the text. Only the top surface of the text should be highlighted.
3c) Hold down the SHIFT key and click on the flat surface where the text starts. (not the back surface of the first block feature, the front one)
3d)let go of the shift key, and all the surface of the text should be highlighted.
3e)While all the text surfaces are still selected, press the control key, and click on the top surface of the text. This should unselect the top surface of the text.
3f) go the the references tab in the dashboard. Click in the draft hinges box and select the top surface of the text, and specify the angle. (ex 10deg.) and complete the feature.

This was the difficult part.

Now we have the extrusion at the top.
You could even use this part now as a punch for the sheetmetal option, or ....

4) Follow steps 3a to 3d again. (Im not typing them again

)
5) With the text surfaces still selected, Hold down control and click the surface mentioned in 3C again to add it to the selection. You should now have all the text surfaces selected as well as the surface where text extrudes from.
6) Click on COPY icon.
7) Click on PASTE icon.
8) With feature still selected click on EDIT, OFFSET.
9) Change direction to the back if required, and add value of 1 for offset and complete the feature.
10) With the feature still selected, click on EDIT SOLIDIFY and complete the feature.. (The block is step was made thicker so that this surface cut has some solid geometry to cut)

No the text in the second feature can change or the text can be linked to a parameter. And this could then be used in a family table.

 

[mstols]

I made some movies of the steps. I've you cannot play it Download the techsmith codec. at http://www.techsmith.com/download/codecs.asp.



2008-11-24_125200_1.zip
2008-11-24_131051_2.zip
2008-11-24_131246_3.zip

 

[rudresh.hm]

option1: use surface to create the geometry and thicken
the surface.
to creat the surface i prefer to go with drafter offset
tool. for sketching the text which needs to be varied in
the instances, we can use a string parameter to enter
the variable values in family table and call this
parameter in the sketcher. this will automatically
change the sketch text with respect to the instance.

optio2:like many people are suggesting to use sheet
metal module and suggesting to use punch/die to create
embosing, i will also agree with this method.
the punch text can be controlled using family table
string parameter as described above.

in both the cases we need just the parameters to be
entered in the family table.

i prefer the above two methods over using a protrusion
on one side and cut on the other side, because if the
thickness of the sheet metal used is to be varied the
sketched need to be reworked to alter the offset values.
the above two methods ensure uniform wall thickness,
even when the wall thickness is varied in the instances.

 

[michaelpaul]

over using a protrusion
on one side and cut on the other side, because if the

thickness of the sheet metal used is to be varied the

sketched need to be reworked to alter the offset values.

Assuming that the base thickness is equal to the thickness of the embossed lettering, you can also create the base at X thickness and then create your text offset by X thickness. Then create a shell and select the back surface and make your shell thickness X.

Granted, it's two variables that you have to create but you could set up a relation so you only ever have to change one of them.

Just another way to do it. Not saying it's the most elegant.

Michael

 

[mstols]

rudresh.hm

I see a problem with your way of just offsetting a surface. The problem is that the text option is not available when using the offset surface tool. You can have an external sketch with text, and reference that with the use edge option, in the offset surface.

The problem is that the used edges won't update automatically if the text is changed, manually or with a parameter. (or am I missing something) Please explain how you would get the offset to update if the text changes. Or even better, upload a simple part if possible

 

[mstols]

das_thunder,

Here is another easy way.

Create a solid block. Create the text on the top surface as a solid. Draft the text.

Create a shell feature. Select the back surface to be removed, as well as the four surrounding surfaces of the block.

This will leave the top surface and the text behind and the part will be constant thickness

 

[swf-1]

Srinivasanyeri,


Can you explain in more detail, the second paragraph of your reply above.


If you want to do it in solid.... click on the 3D models
at the top of the page which will take you to
traceparts..where you will get embossed texts.
I hope this helps



Specifically "click on 3d models" I'm using WF3 and I see nothing at the top of the page thathas a command"3d models"


Thanks,


Steve

 

[rudresh.hm]

rudresh.hm

I see a problem with your way of just offsetting a surface. The problem is that the text option is not available when using the offset surface tool. You can have an external sketch with text, and reference that with the use edge option, in the offset surface.

The problem is that the used edges won't update automatically if the text is changed, manually or with a parameter. (or am I missing something) Please explain how you would get the offset to update if the text changes. Or even better, upload a simple part if possible

@mstols,


yes you are right! i missed that one point. i think pro/E needs this enhancement! i dont understand why they have removed this(sketch text) in the sketcher of offset feature.


alternately, we can use extrude surface with capped ends and merge with the base/flat. for draft and fillet, we can use use intent chain. this works I have done it.


as many others are suggesting we can very well go for shell. this maintains the draft angles and relations of inside to outside radii.
Edited by: rudresh.hm

 

[SRINIVASANIYER1]

Specifically "click on 3d models"