Glenn Schroeder

FAQ - Part 2

Discussion created by Glenn Schroeder on Jan 11, 2017
Latest reply on Jan 16, 2018 by Jim Wilkinson
Branched to a new discussion

Frequently Asked Forum Questions (see attached PDF) has 25 topics, and I think that's enough without it getting too difficult to navigate, so I'm starting a new one.  To avoid confusion I'll start here with #26.  I'll add to and edit this periodically, and if you see a mistake or have a suggestion please send me a Private Message.  I really hate typos.

 

2018-01-16 edit:  I'm happy to report that as of today there is a blog section of the forum dedicated to FAQs.  Please see it here: FAQs (Frequently Asked Questions).  Most of these topics are covered there.  Because this new section will be much easier to navigate I will no longer be editing or adding to these two Discussions, but I will leave them in place since they've been linked to from so many other Discussions.

 

26.  Saving document settings

27.  SW on a Mac

28.  Placing holes on a cylinder or cylindrical surface

29.  Drawing dimension lost reference

30.  Using an Equation or Global Variable in a feature

31.  What does this icon mean?

32.  Can I get some help with my schoolwork?

33.  Moving sketch from Assembly to Part

34.  Dimensioning to the intersection of two edges

35.  Saving a Drawing or Assembly to make changes

36.  Using one Part to remove material from another one in an Assembly

37.  Removing unwanted Part from new Assembly

38.  Assigning different Materials to bodies in a single Part

 

   26.  I've made some changes to a Part at Tools > Options > Document Properties, but when I start a new Part it reverts to the default settings.  How can I use those in a new Part?

   (Before I get started, the instructions I'm giving here apply to Parts, but the process is the same for Assemblies and Drawings.)

   Open a new blank Part and make the desired changes.  Go to File > Save, and choose Part Templates (*.prtdot) from the drop-down at "Save as type:".

 

   Name the file appropriately and save.  I'd strongly suggest saving it somewhere other than the default location in the SolidWorks installation folder so you won't lose it if you upgrade to a newer version.  If you're in a multi-user environment you might want to save it to a network so it's available for other users.  Next go to Tools > Options > System Options > File Locations > Document Templates.

 

 

   Click on the "Add..." button, browse to the folder where you saved the template, and select it.  I'd suggest deleting the default location that's there now, but that's up to you.  Now when you start a new Part you should have the new template available to choose from.  If you don't, and you see this...

 

 

...which only has the default templates to choose from, click on the "Advanced" button at lower left.  Then it should look something like this:

 

 

You only see one Part and one Assembly template here because that's all I need.  Depending on your needs you can certainly have more.  Just name them appropriately so you know what you're choosing.  If you have a large number of document templates you can add sub-folders at the location you're pointing to at File Locations > Document Templates and these sub-folders will show up as tabs in the Advanced New Document dialog box.  See above.  "Templates" is my main folder that contains all my templates, and "Other Drawings" is a sub-folder.  It contains some drawing templates that I rarely use but don't want to get rid of.

   While I'm on the subject, occasionally someone will ask how to apply new Document Property settings to an existing document.  You can open a document with the desired settings, go to Tools > Options > Document Properties > Drafting Standard, and select "Save to External File...".  Save this standard, then open the model or drawing you want to update, go to the same location, choose "Load From External File...", and Browse to and select the desired saved standard.  I haven't used this much, and have gotten mixed results when I did, but it's worth a shot.  Another option, for Drawings, is to open the existing Drawing, then start a new one with the new Template, and copy sheets from the existing document and paste them into the new one.  This isn't a perfect procedure either, but one I've used with some success.

 

 

   27.  Can I use SolidWorks with my Mac computer, or does it only run on Windows?

   See the reply from Anna Wood at what is the best way to run SW on a Mac laptop? I have nothing to add as I have exactly zero experience with Apple products.

 

   28.  I want to place some holes on the surface of a cylinder.  How do I do that?

   If you need simple round holes, slots, or any other type that can be made with the Hole Wizard feature, it's pretty simple.  When you place the sketch points to select the locations the holes will be perpendicular to the cylinder's axis.  For any other feature I'd suggest creating a plane, and then use this for a 2d sketch just like you'd do for placing holes on a flat surface.  You'll need two references to fully define the new plane.  The simplest is to use the cylindrical surface (Tangent) and another plane (Parallel, Perpendicular, etc).  If using an existing plane doesn't work then you'll probably need to create a sketch and use one of its entities (line, point, etc.) for the second reference.

 

   29.  I made some changes to my model, and when I went back to the Drawing one (or some) of the dimensions have turned an ugly yellowish-brown color.  What happened and how can I fix it?

   That's referred to as a "dangling dimension", meaning it's lost its reference to the model  Either it was referencing something that's no longer there, or something that's moved, or maybe your computer just hiccuped.  If it had referenced a feature that was deleted then you'll obviously need to click on the dimension and delete it.  If its reference just moved, you should be able to re-attach it.  Click on the dimension to highlight it.  There should be a small red box at the end of an extension line.

 

 

   You should be able to click on it and drag it to the new reference.  Keep in mind that you can only re-attach it to the same type of reference that was used to create the dimension.  For example, if a model edge was used to create the dimension then you won't be able to re-attach it to a point or vertex.  If you can't get it to re-attach, which sometimes happens, just delete the dimension and use the Smart Dimension tool to insert a new one.  Occasionally a dangling dimension will appear to not be selectable (won't turn blue when you click on it), but when that happens I've always been able to click on it anyway and delete it with the Delete key on my keyboard.  I've also run into a situation a time or two when a dimension would turn that color and appear to have lost it's references, but would be all blue when I clicked on it instead of having the red box.  This seems to happen mostly when copying and pasting sheets from one drawing to another.  When that happens I can still click on the box at the end of the extension line and re-attach it.

   While I'm on the subject, notes and balloons (and other annotations) will sometimes lose their reference also and turn that same color.  When that happens just click the end of the leader and re-attach it.  The leader may still look like it's attached, but grab it and move it just a little bit.  That should fix it.

   There's a setting you can choose that will automatically hide these annotations, but I keep it turned off.  If there's a problem with an annotation I want to know about it.  If it just goes "poof" I very likely might not notice.

 

 

   30.  I have a Global Variable (or Custom Property, etc) that I'd like to link to in a Linear Pattern, Distance Mate, or similar feature that contains a dimension.  Is this possible?

   Yes.  Some features, such as Linear Component Patterns in Assemblies, allow the use of Equations directly in the Property Manager (just type the Equal sign in the dimension dialog box, see below), but this was added fairly recently, so may not be available if you're using an earlier version, and still isn't available for all features.

 

   If you can't do it directly in the Property Manager, go ahead and create the feature, using a dimension that's close to what you need.  Click Okay to close the feature, then single-click on it in the tree to show the dimension in the graphics area (or double-click if you don't have Instant 3d turned on).

 

 

   Double-click on it to bring up the standard dimension dialog box, enter the Equal sign, and link to your variable, custom property, etc.  You'll need to do a manual rebuild for the change to take effect.

 

 

   31.  I have an icon in my tree that I don't recognize.  What does it mean?

   Please see this blog post from Jim Wilkinson.  It shows all the icons (or almost all; if you have one you don't see there please let him know), along with links to SW Help for each group.

 

   32.  I'm having problems with a school assignment.  Can someone help please?

  I, or someone else, will be glad to help.  Most of us here enjoy helping others learn more about SolidWorks, and some active forum members are teachers.  If you want help learning then please post your specific question about what part of your assignment you're having trouble with.  Include screenshots of your work at a minimum, and attaching your model will be better.  More and better information will get you more and better answers.

   If, on the other hand, instead of help you want someone to do your work for you, please don't bother asking.  It's dishonest, you won't learn anything that way, and we have better things to do with our time.

 

   33.  I have a sketch that was created in my Assembly, and I'd like to move it to one of the Parts in the Assembly.  Can I do that?

   There isn't a way to do that directly, but there are at least two methods that should work for you.  You can copy the sketch from the Assembly and paste it into the Part file, then delete it from the Assembly.  You will need to reapply some relations to fully define it in the Part.  Another option would be to edit the Part within the Assembly, create a new sketch on the same plane as the Assembly sketch (or one that's parallel to it), and use the "Convert Entities" sketch tool to reproduce the sketch entities in the Part.  If you use this option you will of course need to keep the sketch in the Assembly instead of deleting it, unless you first delete the "On Edge" relations.

 

   34.   How do I dimension to the intersection of two edges, such as at a chamfer or fillet?

   With the Smart Dimension tool active, right-click on one of the edges and choose "Find Intersection" from the drop-down.

 

 

Then click on the second edge.  That will insert a Virtual Sharp at the intersection of the two edges, and establish it as the dimension reference.  This right-click option is a fairly recent enhancement (SW2015, maybe?).  If you're using an older version, then exit the Smart Dimension function, Ctrl+select the two edges, and then select the Point sketch tool.  That will place a Virtual Sharp at the intersection of the edges, and now you can dimension to it.  By the way, you can choose which of several styles you prefer for Virtual Sharps at Tools > Options > Document Properties > Virtual Sharps.

 

 

Unfortunately, there isn't currently (as of SW2017) a way to set a Layer or color for them.  You can use a Layer to change the color if you don't like the default.

 

 

   35.   I have an Assembly (or Drawing), and now I want a new one that's very similar.  What's the best way to do that without messing up the original?

With the parent file open, go to File > Pack and Go.  That will allow you to copy the file, and all of its dependent files (Parts, sub-assemblies, etc.) to another location.  Most of the options are self-explanatory, but I'll touch on a couple of them.  If you use Toolbox, there's a box near the top left you can de-select to avoid copying them.  There's also an option near the bottom left to send the files to a Zip file, which is handy if you need to send them to someone (or post them in a forum).

 

Changing the names of the new files is a good policy to make sure you don't get unintended changes to your original files.  There are three ways to do this:

   1.  Double-click on the file name in the "Save to Name" column.  That will allow you to assign a new name to individual files.  This works fine if there aren't too many files, but for those with quite a few use 2 or 3.

   2.  There are checkboxes near the bottom right corner where you can add a suffix or prefix to the new file names.

   3.  Use the "Select / Replace" button (near the center, just below the list of files) to replace text in file names (such as project numbers) with new text.  This function can also be used to exclude some components (such as library parts) by selecting "In Folder" from the Search drop-down, entering a key word, and then selecting "Uncheck item(s)".

 

When you've finished and clicked "Save", be sure to close your original file, then open the new files to make your changes (I learned this the hard way).

 

   36.   I have one Part interfering with another one in an Assembly and I want to use the interference to remove material from one of them.  How do I do that?

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.

 

 

   37.   When I start a new Assembly there is a Part (or Parts, or a sketch, etc) already there that I don't want.  What happened, and how do I fix it?

Somehow your Template got saved with the Part in it.  Possibly you (or someone) started a new Assembly, made some changes at Tools > Options > Document Properties, and saved the template after this Part had been inserted.  How it happened doesn't really matter, but it's easy enough to fix.  Start a new Assembly with this template, delete the unwanted item, and then File > Save as > Assembly Template.   Saving it to the same name will override the template with the item inserted, or save it to a new name.

 

   38.   I have a multi-body Part, and I'd like to assign a different Material to one (or some) of the bodies.  Is that possible?

Yes.  Expand your Cut list folder all the way down to the body name.  Right-click on it and Material should be there in the drop-down menu.  After that it works just like selecting Material further down in the tree.  If it's not there, then just like on pretty much every other SolidWorks right-click drop-down click on the little double-arrows at the bottom to get all available options.

 

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