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Silkscreen - AGAIN

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Message 1 of 17
tmoxam
1521 Views, 16 Replies

Silkscreen - AGAIN

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?

Tim Moxam - Senior Mechanical Designer
Windows 7 64 bit
Inventor 2012 Professional
Dell T1600 CPU E31245 @ 3.30GHz
8 GB RAM
16 REPLIES 16
Message 2 of 17
jletcher
in reply to: tmoxam

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

Why NOT.JPG

 

This is with part line visibility off

 

Off.JPG

Message 3 of 17
tmoxam
in reply to: jletcher

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.

Tim Moxam - Senior Mechanical Designer
Windows 7 64 bit
Inventor 2012 Professional
Dell T1600 CPU E31245 @ 3.30GHz
8 GB RAM
Message 4 of 17
Ryan.Martinez
in reply to: tmoxam

Untitled.png

 

Like this?

P.D.S. 2015
P.D.S. 2016
Message 5 of 17
jletcher
in reply to: tmoxam

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....Smiley Happy

Message 6 of 17
mcgyvr
in reply to: tmoxam


@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.


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.

 



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Message 7 of 17
tmoxam
in reply to: mcgyvr

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,

Tim Moxam - Senior Mechanical Designer
Windows 7 64 bit
Inventor 2012 Professional
Dell T1600 CPU E31245 @ 3.30GHz
8 GB RAM
Message 8 of 17
jletcher
in reply to: tmoxam

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

 

Associative.JPG

Message 9 of 17
tmoxam
in reply to: jletcher

Yaaaaaay!!

Tim Moxam - Senior Mechanical Designer
Windows 7 64 bit
Inventor 2012 Professional
Dell T1600 CPU E31245 @ 3.30GHz
8 GB RAM
Message 10 of 17
Toddjfw
in reply to: tmoxam

Our company recently made the switch from Autocad to Inventor 2013 and this thread has been VERY helpful in getting our silkscreening to show up on our 2D drawings, so thank you all very much.

 

One little glitch we're having is that we sometimes include an isometric view on the drawings and haven't found a way to get the silkscreening sketch to show up in that view. Any suggestions?

 

Message 11 of 17
Toddjfw
in reply to: Toddjfw

I'm attaching an image to show the problem.

 

 SCREENING.png

Message 12 of 17
jletcher
in reply to: Toddjfw

You are correct in an ISO view you cannot retrive the sketch don't know why but it might have been over looked when they added the option.

 

For you I would suggest a new route.

 

 I would create a derived part use the part you need the silk screen on and make it a phantom so it does not show up on the bill of materials.

 

my.JPG

 

Message 13 of 17
tmoney2007
in reply to: tmoxam

I usually set up my views in the assembly before I start the drawing.  It tends to be much easier that way.

 

Someone should request silk screening as a feature.

Message 14 of 17
Toddjfw
in reply to: jletcher

Thanks for the replies.  I apologize for my delayed response.

 

James - We have covers that are used on multiple models. The part is the same, but the screening is different for each one. Do the derived parts exist only in the part drawings (IPT) or are they separate files that we would need to store somewhere else? We don't use the BOM function, so making is a phantom part isn't a concern.

 

Also, how did you make that silk screening? Emboss, extrude, or is that a sketch?

 

Tmoney - A feature would be great. Or even an Add-In maybe.

I don't understand what you mean by setting up the views in your assembly. Does that make your screening sketch show up in an ISO view? Sorry, I'm still fairly new to Inventor.

Message 15 of 17
jletcher
in reply to: Toddjfw

No need to apologize it is on your time.. Take a look at this assembly I made may help you understand..

 

Here is the issue with a silkscreen feature. There are many companies and each handle silkscreen different then the other. For a regular shop you can show the silkscreen with the part. But in the DOD you must have a separate drawing for the part and silkscreen. So what I do because of DOD is the assembly attached. The assembly here is not named the same as the part but in some cases I do name the assembly and the lid the same and hide the part in the BOM and use the assembly for the callout.

 

Now you say you have same lid but different silkscreen so you would need a few assemblies to do this but that is the way it should be anyway if you ask me. But you could have one assembly and many silkscreen and just suppress the one you don't need with LOD.

 

There are many ways to handle it you will have to figure what one works for you..

 

The file is a zip file

 

Let me know if you need anything else..

Message 16 of 17
Toddjfw
in reply to: jletcher

Thank you very much James.

That was above and beyond the call of duty!

 

The samples were very helpful.

We got it figured out and that is now our "company policy". Smiley Happy

Message 17 of 17
jletcher
in reply to: Toddjfw

Your welcome glad I could help..

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