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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.