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2018

In the Assembly, click on the one you want to cut and choose the "Edit Part" icon.  That will allow you to edit this Part in the context of the Assembly.

 

 

Now choose the Indent command (Insert > Features > Indent).  Select the Part you want to cut ("Target body:") and the Part you want to cut it with (Tool body region:), and choose "Cut".

 

 

Click on the Okay icon and you're done.

 

In most cases, sketch entities are shown with a thick line font, but sometimes, you will see some of the entities with a thin line font. The image below shows examples of these thin entities:

ThinSketchLines.png

In early versions of SOLIDWORKS, all features required the use of a single "contour" (a single loop of connected sketch entities) to be used to create a feature. In current versions of SOLIDWORKS, some features still require single closed contours. Therefore, there are algorithms in the sketcher to highlight cases where the entities do not form a single closed contour since these entities often are created by mistake or will cause problems in downstream features if not corrected. The sketcher tries to display entities that DO NOT form part of a single closed contour in a thinner line font.

 

Which entities display as thin line font often depends on the entity creation order and also how the entities connect to vertices of the entities that are part of the single closed contour. For example, the first two squares in the image above show different lines in the thin font even though the geometry is the same. This is because of the entity creation order. In the bottom case, the line on the right is shown as thin because it connects to the outer closed contour at a vertex/endpoint. All of the other lines connect to the single contour in the middle of other lines, not at the vertices/endpoints and the algorithm is not designed to highlight these cases.

 

Depending on the usage of the sketch, the user may not care if there is a single contour in the sketch or not so the thin lines can simply be ignored in these a cases. An example of this is if the user us going to use the contour selection tool to identify which contours will be used for the particular feature.

If your Assembly shows some components suppressed and you can't un-suppress them, or if your Drawing is showing dotted line boxes instead of your drawing views, then it's lost the link to the dependent files. You or a coworker may have improperly moved or re-named the files, or maybe you received the file from someone else and he or she didn't send all the dependent files. Assuming it's the first of those examples, and assuming you know where the files were moved to (or what they got re-named to), it's easy enough to restore the links. One method is to close the file and go to File > Open. Browse to the file and select it so it's highlighted, but don't open it. Click on the "References" button.

 

 

That will open another dialog box, with all dependent files listed, along with their folder locations.

 

 

If the file was renamed then double-click on the file name and select the new name from the Browse dialog box. If it was moved then double-click on the folder name string instead and Browse to the new location. If more than one reference was lost you'll need to do this for each one.

 

For Assemblies, there's another method that you might want to try. As I said above, if SW has lost the reference to components then they'll come in suppressed. You can try to click on them and choose the "Unsuppress" icon. Prior to SW2018 when doing this I'd get a message box asking if I wanted to find the component myself, so I could browse to and select it, and it worked fine. However, maybe it's just me, but starting with SW2018 I don't always get that message box. Nothing happens when I try to unsuppress. However, I've learned that I can open the Part, then go back to the Assembly, and I can unsuppress. If that component had been patterned then the pattern will likely show an error (see below). You can manually suppress the pattern and then unsuppress it, or expand it and unsuppress the components, and the error will go away.

 

 

In the future, if you want to move or rename files while maintaining the links do so in SolidWorks Explorer, or right-click on the file name in Windows Explorer and choose SolidWorks > Rename... (or Move...). However, this option will only be available if you have SolidWorks Explorer installed. Depending on your Search parameters this might also not find all references.

 

 

Beginning with SW2016, another alternative for Assemblies is renaming the dependent files directly in the Assembly (see here). I've had good luck with this option. I have fond hopes that at some point in the future we'll be able to use a similar workflow to rename files from a Drawing, but so far (as of SW2018) that's not available.