Lines missing in isometric views

Good Morning!

I, and the people in my office, have had a recurring issue with some of our isometric drawing views. When placed, the views have missing lines. It happens when they are pulled from other views and the missing lines change depending on the view pulled from. We've tried making the drawing for the same assemblies/parts on other computers with the same issue. Any help would be greatly appreciated.

Thanks,


Trevor

Here is a picture!

SolidworksDrawings And Detailing
Answers 9
JM
JM 2013-12-10 Best Answer

If you move your cursor over the missing line's location, is it there?

Now for the tough questions, what graphics card(s) are you using and are the drivers SolidWorks approved?

SF
SF 2013-12-10

Yes, the lines do exist and can be selected to do things with(tried hiding then unhiding to no avail), they just are missing.

We checked our graphics cards ths morning and they appear to be solidworks approved.

Thanks for your response.

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GS
GS 2013-12-10

Have you tried switching back and forth between display types (Hidden Lines Shown, Hidden Lines Removed, etc.) for that view?

SF
SF 2013-12-10

Yeah, they show up in every other view type but the type we need.


Thanks

JM
JM 2013-12-10

While the card is approved, what about the driver? I've had instances where a Dell update will change the driver.

GS
GS 2013-12-10

Have you tried a Ctrl+Q rebuild?

JB
JB 2013-12-10

I ran into this issue on drawings of large models a lot-and coincidentally my machine was a T3500 with a Quadro FX3800 video card.

Annecdotally, I can tell you it appeared to be dependent on the number of edges SolidWorks had to draw-which included edges on sheets other than the active one.  This was a big problem when it came time to export drawings as PDF's.  In one case, the only way to get the sheet to render correctly was to hide views on the other sheets, render the problem sheet seperately and then use Acrobat Pro to combine the files.

Most of the time, I tried to use shaded with edges mode, so that the missing segments wouldn't make the drawing difficult to understand.

The other thing I could try was hiding the view and unhiding it, forcing SolidWorks to redraw it.

Now, there's a difference in causes between what I've described and having edges disappearing in cases where the geometry containign the edge interfered with other geometry in the assembly. In those cases, the answer is to resolve the interfereces.

In 2011 and later, there's an option the PDF export dialog box to use high-quality lines when exporting PDF's to make sure that close or thin line segments weren't skipped.

Final thing, make sure you're running the latest service pack for Windows 7.  I seem to remember that the initial release had a maximum number of GDI handles of 10000 which produced some display problems for SolidWorks.  SP1 for Windows 7 resolved this issue, I believe.

SF
SF 2013-12-20

We updated to the newest drivers and it seems to have fixed the issues. It just took forever for IT to get around to it.

Thanks Everyone!

KH
KH 2013-12-20

Trevor,

Another thing to think about is interferences. If components have interferences the edges are sometime displayed incorrectly depending on your display type. Also make sure the view is set to high quality.

Kevin