Go to OPTIONS, Document Properties, Line Style.
New, name the new line syle i.e. NONE, then A,-1,-1.
Then go to OPTIONS, Document Properties, View Labels, Detail, then set your detail and border to the blank line you just created.
Hope this helps!
Oh, and just to warn you, there will be a dashed line on your drawings as a guide, but this disappears when you print your drawing.
Creating a crop view is a work around. I was hoping for a simple "hide border" button ???
This seems like a good solution. I was able to create a new line type and the preview window shows a "blank" line. Then I assigned this linetype to detail and border. When I create my new detail view, I get a DASHED type line??? I am running SW2008 sp4. Please see attached files...one file linetype is blank and one is named none. I had tried both names sparately.
David, as per Jennifer there will be a dashed line on your drawings as a guide, but this disappears when you print your drawing. Did you tried a test print?
Jennifer, thanks for the cool tip
I guess the next question is, can we do this for just one detail while keeping other details with standard lines?
I don't see what's wrong with just doing a crop view. It's super easy and doesn't affect other detail views.
crop is ok but if the view is single and separated but some times you need to link the view with another which is existing already.
in this case if you modify something like changing the configuration you need to change it again in the crop view but if link it to parent view by using detail sketch, no need to do this step
Thanks Jennifer, that's just the trick I needed for hiding the border of detail views.
I found greater success making my line format A,-0.0001,-10000 This makes the line very short and the space very long.
Using this line setting the line around detail views completely disappears (it's not even there as a 'guide'). 'Save as PDF' now also works correctly, no need to print to PDF to get the correct results.
I did the same thing as Keith and it works great!
Great post very helpful. Is it possible to do it for only one detailed view?
I find it a lot easier to just create a new layer and call it "detail circles" and then put the circles in that layer and turn it off.
Another option would be to put the detail circle on a hidden layer. I tried this and at first it didnt disappear but when i toggled the visibility of my hidden layer to visible and then back to hidden it worked fine.
Yes, This is better and easier. thank you Mr Eddie and Blair
Right click on the circle > Change Layer, the choose your hidden Layer
To make a layer hidden just go to line format tape > Layer Properties > On/Off the layer
if line format tape is not appear in your solidwork just click one right click on any tape you need (view layout annotation sketch evaluate ... etc) the select the line format tape
And with SolidWorks 2015 the Layer may be hidden only during printing.
A trick I have used for years (even before I started using Solidworks) is to make a duplicate view and use only the lines you want and hide the ones you don't.
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