Drawing Isometric view SHADED

Hello All,
I'm wondering if any one has any experience with using shaded ISO views. I'm having a problem with the line thickness displayed and plotted. I could not find any area for changing the thickness of ISO Shaded views. Under document properties-line font, there are options to change thickness of lines, however it doesn't seem to affect the ISO view. Even if I change a standard projected view to shaded, and then change the line thickness they change, but not the ISO view. Am I missing something? I did call our VAR (creative design concepts) and they suggested I send an email, which they can forward onto Solidworks. I don't mind going this route, however I get the feeling I will have better response this way. Any info is greatly appreciated.
Regards, Pete

Try this.
Click File>Print>Page Setup Under Resolution and Scale, check High Quality
It will take a LOT longer to print (a major printing peeve of mine), but should output good edge line thicknesses. When doing this however, if you have any headers or footers on your document, they will not print (yes, yet another printing peeve of mine).

I printed a lot of shaded ISO-views ....at least in SW 2004 without any problems....haven't tried it 2005 yet due to the increasing plotting time. On the other hand I don't pay that much attention to line thicknes in ISO views as I do in the normal views....as long as it looks okay.
Krister L
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Pete, I print shaded ISO views often and I am not very happy with how SW2005 treats visible edges color. Visible model edges in my regular views need to be red, but in ISO views I need edges black. In SW2004 I used Options-Colors, Drawings Visible Model Edges and set the color to red. It used to affect regular views only, not the ISO views, which remained black. SW2005 affects both!!! I have to put ISO views on separate sheet and change print settings for these sheets. What a pain...
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I have an idea. I don't use SW2005 yet so I don't know if it will work.
1. Create a layer with the color property set to black. 2. Right click on your iso view and select "Component Line Font". You may have to click the arrows at the bottom of the menu to get this list item. 3. In the "Component Line Font" dialog, uncheck "Use document defaults". 4. Under Drawing view, check "From selection". 5. Then select the new layer your created in the layer box.
What happens? If this doesn't work immediately, try rebuilding. Did that get it? In SW2004, I can NOT get this to work like you would expect it to. But since it sounds as though SW2005 works opposite than SW2004 for you, then it just might work.

Seth, I tried your suggestion - it works in 2005! The important thing is to remember to check "From selection". Now I don't have to print iso sheets separately. However, I didn't have to do it in 2004. On the brighter side, Pete, you can control line thickness in the same Component Line Font dialog box.
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zz, Glad to hear it. You might be able to set up your templates with this new, black layer, as well as a predefined iso view with this adjustment already made in the Component Line Font dialog. This would prevent you from having to go through this process on every new drawing.

Pete,
Select the ISO view in your drawing and check to be sure that the "High quality" button is checked in the "Display Style" box in the feature manager tree.
HTH,
M.T.
On 14 Oct 2004 08:36:06 -0700, snipped-for-privacy@gmail.com wrote:
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