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This is a broad topic, but I'll try to address several possibilities. One thing to keep in mind is that when you start a pattern or mirror feature, "Features and Faces" (red arrow below) will be selected by default, and the first box (Features to Pattern) will be active. See the screenshot below. You'll see why that's important further down when I discuss specific situations. Also, for some reason unknown to me, the number of instances (third box down from the top, with 2 in it) includes the seed that's being patterned, so in the example below one new feature would be created. The numeral 1 is there by default on some occasions. Again, I don't know why, since the feature won't work with 1 entered there.



  • If, for example, you're trying to pattern a single hole that was created as part of a pattern, and the software is trying to pattern all the instances instead of just the one you selected, that's because by default the first box under "Features to Pattern" was active. Clear that box and click in the one below it instead, then select the face of the hole. If it's a rectangular hole you'll need to select all four faces (or five if it doesn't go all the way through the body), etc.


  • Keep the "Geometry pattern" box in mind. When it's not selected then the pattern will use the same conditions as the seed. For example, if you're patterning a hole, and the hole was created with "Offset from Surface" as the end condition, then the patterned holes will maintain the same offset from the same selected face.


If that box is checked then the same exact geometry of the seed feature will be patterned, ignoring the end condition.



  • If you're working with a multi-body Part and trying to pattern a single body or combination of bodies, you'll get better results if you de-select the "Features and Faces" box and select Bodies instead, then select the body or bodies to pattern. Failing to do that is a common mistake. If that's the situation, and you've already created the pattern, you can edit it if you're using SW2015 or later. You'll need to un-check the Features and Faces box and clear it's selections, then proceed with Bodies. If you're using an earlier version you'll need to delete this pattern and create a new one, this time choosing Bodies instead.


  • If you've done that and it's still not working right, make sure this body hasn't been inadvertently merged with another body or bodies. Click on the feature that created the body, select the "Edit feature" icon, and make sure the "Merge bodies" box isn't checked. Since that box will often be checked by default that's also a common mistake.


Speaking of patterns, I never use sketch patterns. I've had better results with creating a single feature or body with the sketch, then patterning it. There may be situations where this isn't true, but I have never run into one. I know there are some people that are hung up on keeping the feature tree as short as possible, but sometimes it pays to have the extra line or two.


Mirroring sketch elements, on the other hand, usually works pretty well, and I do it often.


If none of these address your issue, feel free to post it on the forum as a new Discussion. Please include the Part when you do (see How can I attach a file to a forum post?).

Check the box shown below in the Feature's Property Manager, then choose All components or Selected components.  If you choose Selected components you will likely need to un-check the box for Auto-select, and then choose which Part files you want the feature to propagate to.


Also keep in mind that if you choose "All components" it will affect components that are added after the feature.  I found this out the hard way (it took me longer than it should have to figure out why my washer didn't look right after it was mated to the hole).


Yes, the Copy Settings Wizard will do that.  It will let you save a file with all your toolbars, menu selections, and other workspace settings, along with your settings at Tools > Options > System Options.  You can then go back to the Copy Settings Wizard to load these settings when needed.  While it's perfectly fine to save this file to your hard drive, I'd suggest keeping a backup on a network, flash drive, etc. in case your computer dies, or for when you get a new one.  And it doesn't automatically update, so to keep it current you need to save a file every time you make changes.  Please keep in mind that some experienced users recommend not using the Copy Settings Wizard to restore settings when upgrading to a new version, but instead set up everything manually.  I've personally never had any problems with it, but it's something to keep in mind.


There are several ways to get to it.  If you have SW open, you can go to Tools > Save/Restore Settings...



...or go to the SolidWorks Resources tab on the Task Pane and choose Copy Settings Wizard in the SolidWorks Tools section.



If you don't have SW open you can get to it by going to Start > All Programs > SolidWorks > SolidWorks Tools > Copy Settings Wizard.


To start off, you have to be in the Discussion itself. You can't attach files when replying to a Discussion from your Inbox (thank you Dan Pihlaja for pointing that out).


If you're attaching a Drawing or Assembly please keep in mind that you also have to attach all referenced files or we won't be able to open it, and don't post these files separately, but do a Pack and Go to a zip file and post that (see How can I create a new Assembly or Drawing similar to an existing one? if you aren't familiar with Pack and Go). If you're posting a Part file it's unlikely that you need to zip it first. Just post it directly. And don't attach .rar files. Very few people will open them. I know I won't.


Now that I have that out of the way, if this is in a Reply to an existing Discussion, click on the black text "Use advanced editor" in the right corner above the text box. I know it doesn't look like a link, but it is.



After clicking on that you'll get a link to attach files in the lower left corner. Click on the "Attach" link and Browse to and select the file.


If instead of a Reply this is a Discussion you're just starting, the "Attach" link should already be there. If you've already posted the Discussion and would like to go back and add a file to the original post, click on the "Edit" link near the top right of your original post to get the "Attach" link back.



2018-09-12 edit: If you only want to attach a screenshot you also need to use the advanced editor to post a jpeg or similar file, but there's an easier way. My usual procedure is to hit the PrtScn/SyRq button on my keyboard to copy whatever's on my monitor. Next I open Paint and hit Ctrl + V to paste the screenshot. I use the tools in Paint to underline, point an arrow at something, etc, then use the Select tool to choose a specific area. Ctrl + C to copy it, then go to the open forum post and Ctrl + V to paste it directly in with the text. It's that simple. Other users have somewhat different workflows that I'm sure work just as well (and they're free to post theirs here if they'd like), but this one works well for me.

As with most things with SolidWorks, there are several ways to do this.  Select the one that works best for you.


I'll start with what I believe is the simplest, and the one I almost always use (I like simple).  When you've selected the model to insert in the drawing, go to the "Select Bodies..." button in the drawing view's property manager.



That will take you to the Part file where you can select which body, or combination of bodies, you want to show in the drawing view.  You can also use this feature to add or remove bodies from existing drawing views, not just when creating new ones.


Another method is to insert the drawing view, then right-click on an edge of a body you want to hide and choose Show/Hide > Hide Body.  If you want to get it back just find the body in the tree and right-click on it.  There will be an option in the menu to show it again.



A third option is to save out the bodies as separate Part files by right-clicking on the body and choosing "Insert into New Part..." from the drop-down.  A number of people use this method, but I don't think I've ever had a reason or need to.  If you have to have a separate Drawing for each body because of company standards then you should likely use this method, especially if you have title block notes that are driven by the Part's custom properties.  Unfortunately, at this time title block notes can't be driven by cut list properties. 



Still another option would be to create multiple Display States in your Part, hiding bodies in each as needed, and then reference the appropriate Display State in the Drawing.


Remember I said there are multiple ways to do most things in SolidWorks?  Here's the 5th.  Go ahead and insert a view, then right-click on it and choose Drawing Views > Relative View.



That will take you to the model, where you can choose which faces (or Planes) you want front and right, and you will also have an option to choose which body or bodies you want included in the view.  When you click OK in your model it will place a new drawing view oriented according to your selections.  You can now delete the original view if it's not needed.  Relative View was one method commonly used for showing selected bodies before the Select Bodies... button shown above was added.  I've rarely used it since then, but if you have a body at a weird angle, such as a brace, it can be very useful.

I've seen a number of Discussions here on the Forum about problems when the Windows icon scale is set to anything other than 100% (especially larger, see My layer properties window is not showing the columns for Active layer and On/Off and 2015 Smart Dimension in Sketch Defaults to Dimension ID Entry for just two examples), so if yours is set to something else try switching to 100% and see if that helps.  I believe this is mostly related to not all options being displayed in Property Managers, and in right- or left-click menus.


I've seen a number of people on the forum with graphics issues that were fixed by de-selecting the option shown below, so see if yours is checked, and if yes, de-selected it and see if that helps.



If neither of those help it's very likely to be a problem with your graphics card.  The wrong graphics card, or the wrong driver for the right card, can cause an extraordinary number of strange issues.  Since Windows 10 came out I seem to have seen more issues reported here, and many of them seem to have come from automatic Windows updates, which include graphics card drive updates, causing problems.  Reverting to the previous driver often seems to fix the problem.


Some people use unapproved cards with no problem, but if you're having issues you apparently aren't lucky enough to be one of those.  If you have a company IT person that spec'ed your new machine with a high end gaming card because he/she just assumed it would work well with SolidWorks, you have my sympathies.  Get an AMD FirePro or an NVIDIA Quadro (which is what I use) for best results.  If you already have one of those, check here to make sure you have the correct driver.  The newest driver isn't necessarily the one that works best with SolidWorks.  You might also run the SolidWorks Diagnostics tool at Start > All Programs > SolidWorks 2015 (or whatever year) > Tools > SolidWorks Rx > Diagnostics to see what that shows.


If you have a GeForce card, and it was working fine but stopped, it's probably because of an automatic driver update.  See here.


If you're stuck with a non-approved card, and nothing else works, try selecting "Use software OpenGL" as shown below (Tools > Options > System Options > Performance).  If it's grayed out so you can't select it then close all SW files and try again.  I don't have any experience with this, but I understand that it helps sometimes.  If nothing else, while you may not want to use this long term, if your issues go away while using it then you'll know the problem does lie with your graphics card, so it can be a useful diagnostics tool.



2018-05-25 edit:  I've seen several Discussions on the forum recently from people that were using an unapproved graphics card with no problems, and then Solidworks completely stopped working.  It seems that a driver update was the culprit most, if not all, of the time.  So if that's your situation you might try rolling back to the previous driver.

SW 2016 introduced a thread feature (2016 What's New in SOLIDWORKS - Creating a Cut Thread).  If you're using an earlier version, see Threading Options.  Please keep in mind that while you can create threads, it doesn't necessarily mean you should.  That's adding a lot of surfaces for your computer to have to sort through.  Unless you absolutely need the threads for 3d printing, or for some other reason, I'd recommend not creating them at all.  Even if you are creating a model for 3d printing, I've seen others here recommend cutting the threads after the part is printed for accuracy.  At some point in the future I imagine the 3d printing technology with be able to make accurate threads, but it's my understanding that it isn't there yet.


I rarely create threads.  They can drastically slow down performance, especially if there are multiple instances in an assembly, and even inserting a drawing view of a single Part with threads can slow things down.  I often put a note in my drawings that says something like "Threads not shown for clarity".  If you need threads just for visual effects, then go ahead and make them, but if you're using multiple instances of the Part in an Assembly I'd strongly suggest creating a configuration with the thread feature suppressed, and use this configuration in the Assembly.

If you have a drawing view of a single component, and want Balloons to match a BOM for an Assembly, just right-click on the drawing view of the component and choose "Properties..." from the drop-down.  Check the box for "Link balloon text to specified table", and select the correct table from the drop-down.  After doing that new drawing views will automatically be linked upon insertion if you're using SW2017 or newer, and as long as there's only one BOM in the Drawing (See SW2017 Enhancement That Didn't Make the "What's New" Document).  If you're using an earlier version this will need to be done for each view.


If you have multiple tables in a drawing you might want to name them to avoid confusion when linking drawing views.  To name a table, slow double click on it in the tree, or single-click and hit your F2 key (this also works for drawing views, features in Parts and Assemblies, configurations, display states, planes, etc.)  Naming drawing views and tables may also be helpful if you save drawings as .PDF's, since these names will carry over as Bookmarks.


[2018-08-31 edit:  Beginning with SW 2018, slow double-clicking may or may not work for you for renaming display states (as I understand it, due to fixing a bug that would cause SW to sometimes crash when renaming display states), but single-click and F2 still works.]

The first component (Part or Sub-assembly) inserted into an Assembly is Fixed by default.  It will have (f) in front of the file name in the tree, and it will remain fixed regardless of its position in the tree (if you drag another component above it in the tree it will still be fixed).  If you want to re-position it just right-click on it and choose "Float" from the drop-down.  Now you'll be free to left-click and drag it, hold down the scroll wheel to rotate it, etc., or position it with Mates.  (Placing your cursor on a component, holding down the scroll wheel, and moving the mouse to rotate the component is the default behavior for a standard 3-button or 5-button mouse.  If you have a more elaborate mouse, or have changed the button functions, the behavior may be different.)



By the way, if you placed the first component by clicking in the graphics area, which many users do, then it's position may be more or less random.  Instead you can select the component to insert and then click on the green check mark at the top of the Insert Components Property Manager without clicking in the graphics area. It will then be fixed with it's three primary planes aligned with the Assembly's primary planes.  That's what I almost always do with the first component (and sometimes with later components).  If I don't do that then I immediately Float it and Mate it where I want.  I never just leave a part where it was placed by clicking in the graphics area.


When saving a sketch as a library feature part (.sldlfp file) to be used in the Structural Member function on the Weldments toolbar, it’s necessary to have the sketch selected (so it’s highlighted in the graphics area and has the blue box around it in the tree) when you go to Save as…sldlfp.  That step is commonly over-looked.  After saving the file the Sketch icon will have the green "L" on it if it was saved correctly.



If you've saved the profile sketch correctly and it shows the green L, check the folder you're pointing to at Tools > Options > System Options > File Locations > weldment profiles. Keep in mind that you need to have the correct number of sub-folder levels in this folder, and this will vary depending on whether or not you're using configurations in your weldment profile sketches.  If you aren't using configurations, then your first level of sub-folders will appear in the Standard drop-down (such as ANSI and ISO), the second level will have sub-folders for the profile Types (HSS Square, Angle, Pipe, etc.), and these folders will contain the individual files (left screenshot below).  If you are using configurations then the .sldlfp files will be in the Type folder and you'll choose the desired configuration from the Size drop-down (center screenshot below, HSS Square is the file name).  I use both, so my .sldlfp files with configurations are in the same folder as the sub-folders containing the .sldlfp files that don't have configurations (the right screenshot shows the files in my ansi inch folder).


There are several possibilities


  1. I saw a Discussion here on the forum where a new user was having problems with a company logo disappearing when saving as pdf. He finally realized that the DPI was set to 96. Changing it to a higher value fixed the problem, so check that first (by clicking on the "Options" button in the Save as... dialog box) and see if a higher setting will work for you also.
  2. If that doesn't work, then try printing to pdf instead of saving as pdf. If you can't print to pdf because you don't have the Adobe software, I've seen several people here on the forum recommend Cute PDF, which I understand is a free program that you can download to create PDF's. As a disclaimer, I don't have any personal experience with it, and John Matrishon posted (at Poor PDF Quality - How do I fix it?): "Everyone be aware that CutePDF the free version does not embed the font into the file. This will become a problem if you are using certain viewers to view PDF files, and if the fonts are not compatible. Anytime you are using "print" to pdf, you are not using SOLIDWORKS functions, you are using the software installed locally on your computer. Save AS pdf from inside SOLIDWORKS is your only chance to combat issues related to SOLIDWORKS, so using CutePDF or any other 3rd party printing software may cause you issues. I suggest thoroughly testing all usages. I'm still having to replace PDF files because someone decided to use CutePDF instead, and anyone else with the view reads hieroglyphics where text and dimensions should be."
  3. Maybe the font isn't embedded in the pdf. See why my PDF's Drawings dont save the correct font?; especially the replies from Matt Peneguy.
  4. If you can't save to pdf at all, see if the Reply below from Niklas Johansson at save as pdf not working is applicable to your situation.  Other people have reported problems with other Add-ins (such as the one for this forum) in that same Discussion, so you might try turning off all that you don't absolutely need and see if that fixes the problem.


If you just stumbled across this post and don't know what it's talking about, there's an option to have objects (edges, faces, lines, etc) highlighted when your cursor hovers on them.  It's a tremendous help with knowing what you're about to select before you actually click on it.  I can't (or at least don't want to) imagine using the software without it.  To turn it on go to Tools > Options > System Options > Display/Selection and check the box for “Dynamic highlight from graphics view”.  If you had this turned on, and it turned itself off, it’s almost certainly your 3d mouse.  The 3dconnexion software temporarily turns off dynamic highlighting while the 3d mouse is manipulating a model to prevent multiple edges and faces being highlighted as they move across your cursor.  It's supposed to turn it back on when you release the 3d mouse, and it usually does, but not always.  A few years ago it might happen to me two or three times in a day, then not again for weeks or months, but it's definitely gotten better in recent years.


If it happens to you often enough to be a problem please go to 3dconnexion's technical support site.  I've dealt with them a time or two on other issues and gotten good results.


SolidWorks files can't be opened with an earlier version than the one they were last saved with, and they can't be saved back so an earlier version can open them (except as a dumb solid; see two paragraphs down).  I know that isn't true for many programs, such as Word, Excel, etc., but SolidWorks is many times more complex than these programs, and features may have been created with functions that weren’t available in earlier versions, and there are probably other reasons.  I think Ryan McVay gave one of the best explanations I've seen in the Discussion I link to a few paragraphs down: "Well, because this would require the software to bear the burden of including feature checks, older code, extra code to do the checking and converting, extra Parasolid version exporting, and file restructuring, etc. to exist in the software. Your install DVD just went from 4GB to 10GB- oh crap that doesn’t fit on dvd anymore! And this would only increase every version because you are carrying legacy code and export tools. This is one of the many, but a big reason, why you don’t have backward compatibility across all CAD packages and why users rely on neutral solid exports like STEP and Parasolid- outside of the kernel and 3d definition."


People have been asking for backwards compatibility for years, and maybe someday it will happen, but it hasn’t yet.  Document templates are also not backwards compatible.  If a template was saved with SW2015 you won't be able to start a new drawing, part, etc. with it using SW2014.  Service packs are backwards compatible within the same version.  For example, a file saved with SW2014 service pack 5 can be opened with SW2014 service pack 1.


SW models may be saved as several forms of dumb solids, and then opened with earlier versions, but they will lose the features in the tree.  According to Jim Wilkinson (and he would know), Parasolid is your best option when doing this.  His response at Re: compatibility between versions  was "If you do this, make sure to use Parasolid.  Parasolid is the native format of SOLIDWORKS so there is no translation when going back. STL is DEFINITELY a bad choice because it only transfers tessellated data which is nearly useless compared to the original b-rep solid/surface data."


SW2013 introduced the ability to open files one level newer with service pack 5, and use these files in assemblies, but that has limited functionality (see 2016 SOLIDWORKS Help - Future Version Components in Earlier Releases for more information).  Due to an architectural change in SW2015 that ability was suspended for one year.  It was supposed to be re-instated with SW2016 (see Jody Stiles reply here:Will solidworks 2016 files work with 2015?), but when I checked it didn't seem to be working for me.  I never use it anyway, so it hasn't been an issue for me.


Occasionally someone will ask if there's a way to tell which version was used to save a file if you can't open it.  Yes, there is.  In Windows Explorer, browse to the folder containing the file.  Right-click on a blank space at the top, beside the column names, and choose "More..."



Select "SW Last saved with".




That will add a column indicating which SW version last saved the file.




  By the way, I believe in giving credit where it's due, and I wouldn't want anyone to think I'm smart enough to have figured this out for myself.  I learned about it in a post by Steve Calvert at Can you tell what SW version a model was created with?

Assemblies that have some movement, such as a hydraulic cylinder or hinge, are by default rigid when inserted into another assembly, but they can be made flexible.  Find the sub-assembly in the upper-level assembly tree and click on it.  Choose the "Make Component Flexible" icon.  It should now have the same amount of freedom that it had in it's own file.


I believe this icon was first available with SW 2014.  If you're using an earlier version you will need to choose the “Component Properties…” icon instead.


That will take you to the Component Properties dialog box.  “Rigid” will be selected by default in the “Solve as” section.  Select “Flexible” instead, then “OK”.


By the way, if you have a Limit Mate in your sub-assembly it may be broken when you insert it into the main assembly.  If that happens, delete the Limit Mate from the sub-assembly and apply it in the top level assembly instead.  I rarely use Limit Mates, but I have seen reports on the Forum that this was much improved with SW2016, so if you're using 2016 or later you might give it a try.

Jim Wilkinson

Call for FAQs

Posted by Jim Wilkinson Dec 22, 2017

If you have a suggestion for an FAQ that should be added to this area, post the suggestion as a comment to this post. It will be reviewed and if it is FAQ-worthy, we will add it to the list of FAQs to be added.