Autodesk Inventor

[#1]

We all know there are issues with IDW's and Silkscreens. I don't know why. (after reading 40+ posts back to 2003 you would think AutoDesk would address this)

All i need is to be able to include a sketch with text as a part in an assembly for use in an IDW.

I have done the embossing/decal/extrusion thing, but, the font fill doesn't show up correctly and i am having issues printing to pdf and keeping the font filled properly. When you have 100+ pieces of text extruding each one will take you all day and at the end of it all it still looks crappy.

Although, i use many dimensions on the SS i don't want to see any in the detail view.

I (we all) need to be able to show the silkscreen as simple text with no other parts visible .

So...wishlist....create part with only sketch containing text, no features. Turn off dimensions in sketch. place on IDW.

We are using 2012, soon 2013. Is there no easy solution to this?? Really?

[#2]

What I do is make my text in sketch then show sketch in drawing and hide the model lines of the part.

This is with part border lines showing

This is with part line visibility off

[#3]

I am confused but, how do you show sketch in drawing?

The problem is to have it look correct in IDW. Lets say you have a purchased enclosure that you modify on the front panel to include holes and a silkscreen.

Sheet 1 shows the entire enclosure, sheet 2 shows the modified panel with the hole detail, and sheet 3 shows the silkscreen only. The silkscreen should be part of the panel, that is,that whenever you open the panel the silkscreen is included. it is not a separate file. It also may not be extruded due to the time and file size.( it should just be text )

When i view the assembly on the first sheet, i should see the SS, when i view the panel (hole detail) i don't want to see the SS, and in the SS view i just want to see the text (sketch)

So to use your example i should be able to place the part and then turn off visibility to the part leaving the sketch visible.

HOWEVER, sketches from parts don't show up in IDW. Not even if the only thing in the part is a sketch.

This could be soooooooo simple if Autodesk just allowed the sketch to show as necessary

ALSO,  why can't parts be turned off  in the view browser as in Solidworks, rather than picking and turning individual lines invisible.

[#4 · Accepted solution]

Like this?

[#5 · Accepted solution]

Mine is not a separate file it is in a part with a sketch I did not extrude it. And yes it is a pain to turn of lines but not with filters on and a good window select can't take care of.

Takes me about 6 seconds to turn of part lines to me that's not bad would be faster but I had a smoke....

[#6]

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tmoxam wrote:

ALSO,  why can't parts be turned off  in the view browser as in Solidworks, rather than picking and turning individual lines invisible.

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You can.. BUT you need to uncheck the associative check box (the chain link looking thing) in the base view dialog box..

The intent here is that part visibility should be controlled in the part or assembly file by creating a design view rep.. Or with the box unchecked you can control visibility in the idw without worrying about creating a view rep.

[#7]

I'm sorry Mcgyvr, I'm using 2012 and i dont see any associative symbols in the IDW browser for the view. If i expand the browser I can select a component that i wish not to see in this particular view, RMB, and "Visibility" is stilled grayed out. I wish it wasn't , but, it is.

for the rest of the thread, thank you, i have issued the following procedure for creating silkscreens to our operators and post it here for others with the same issue...

When creating silkscreens when using Inventor I have found the following procedure to work “ as expected” when saving as a pdf.

1.     Create the silkscreen as a separate sketch. DO NOT extrude, emboss, or decal as this is time consuming and a file size waster. Also, fonts shown from these features will not be filled in PDF.

2.     In the browser, under the sketch un-check Dimension Visibility.  This will allow you to use dimensions to control the text position but, they will not show up in the drawing or on the model.

3.     Place the part in a view window in the drawing.

4.     In the IDW browser expand the part you just placed and (RMB) check “ Get model Sketches”. This will turn on the (silkscreen) sketch in the view.

5.     Create a new sketch in the view. (IDW sketch) and place corner “hash marks” and panel dimensions for the panel. ( Using the panel edges as guide) Turn off visibility of this sketch .

6.     Highlight everything in the view window, un-select text (silkscreen) and turn off visibility. Now only silkscreen remains.

7.     Turn on visibility of panel dimensions from 5.

 View now shows proper silkscreen representation.

Cheers,

[#8]

This is the place to uncheck the Associative as Mcgyvr Suggested.

[#9]

Yaaaaaay!!