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2017

With the Smart Dimension function active, hold down your Shift key while selecting the circle.  That will place the dimension to the edge (near or far edge, depending on where you click) instead of the center.  I've occasionally run into situations where I need to reference two arcs or circles with one dimension, such as a slot length, and holding down Shift would only place the dimension to the edge of one of the arcs and the other one would still go to the center point.  When that happens I just accept it, and then change it to Max (see below).

 

If you already placed the dimension, you don't need to delete it.  Just click on it to highlight it and bring up it's PropertyManager, then go to the Leaders tab.  Center will be selected by default, but you can change it to either Min or Max, depending on your needs.  The screenshot below is from a sketch in a Part, but the same principles work with dimensions in a Drawing.

 


This assumes that you were referring to placing a dimension with the Smart Dimension function in a Drawing, or in a sketch in a Part or Assembly.  If you're using the Measure tool from the Evaluate toolbar and want to measure to the edge of a hole or circle instead of to the center, then click on the Arc/Circle Measurements icon and choose the appropriate setting from the drop-down.  Keep in mind that while Center to Center is the default setting, SW will remember your last setting the next time you activate the tool.  It won't go back to the default.

 

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 menu click on the little double-arrows at the bottom to get all available options.

 

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

 

 

Then left 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 SW2018) a way to set a default Layer or color for them in Document Properties.  You can assign a Layer to them after they're placed if you don't like the default.

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.  I can't speak for others, but while I've learned a tremendous amount here, and am still learning, now I mostly just enjoy giving back and helping other users.

 

Now that I have that out of the way, we need you to help us to help you.  Please post a specific question in the Discussion section of the Forum (or in a Reply to your existing Discussion if you were sent here) about what part of your assignment you're having trouble with.  Vague pleas like "Please help" probably won't get much response.  Include screenshots of your work at a minimum, and attaching your model will be better (see How can I attach a file to a forum post? for instructions).  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.  You may find yourself the victim of biting sarcasm, or something like this could happen.

 

Edit:  By the way, if you were sent here and you aren't a student, the above probably still applies.  Give us some more information, show some effort, etc.

Some features allow Equations and linking directly in the Property Manager.  (See 2018 SOLIDWORKS Help - Direct Input of Equations in PropertyManagers for the list.)  It's as simple as typing the Equal sign in the dimension box to get the drop-down where you can make your selection.  See below from a Linear Component Pattern in an Assembly.

 

 

This hasn't always been the case, and still isn't available for all features that use a dimension, but it can still be done.  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 and click Okay to close the feature.  Now there are two options for linking the dimension.

 

1.  Single-click on the feature 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 you'll get the same drop-down shown above.  You'll need to do a manual rebuild for the change to take effect.

 

 

2.  Open your Equations dialog box and go to the "Dimensions" tab.  All dimensions in the model will be listed.  Remove the value in the "Value / Equation" column and enter the Equal sign.  That will give the same options for linking.

 

By the way, I believe in giving credit where it's due.  I just learned about this second option from Frederick Law at Global variables in "Thicken" feature?.

 

When you make changes to the Document Properties those changes only affect the active document.  If you want to apply them to new Parts then 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 described the process for saving a Part template, but it's the same for Assemblies and Drawings.  Just choose the appropriate template type from the drop-down.  I'd strongly suggest saving templates (and sheet formats, and weldment profiles,etc) somewhere other than the default location in the SolidWorks installation folder so you won't lose them if you upgrade to a newer version.  If you're in a multi-user environment you might want to save them on a network so they're 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 have saved.  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 my most used templates, and "Other Drawings" is a sub-folder that 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.  If you're in this situation I'd encourage you to go to Drafting standard refusing to change. Dimension Styles not loading in automatically and view font not changing. What am I doing wrong? .  The first part doesn't pertain to the subject here, but about halfway down (starting with post #7) Dan Pihlaja entered the conversation with some good information.

 

 

For Drawings, another option 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, since it doesn't save all the Document Property settings, but it might work for you.

For a quick change you can go to the bottom of your monitor and make the change with the flyout.

 

 

This flyout is a fairly recent enhancement.  If you're using an earlier version that doesn't have it go to Tools > Options > Document Properties > Units. If you do have the flyout you may need to go there anyway to refine some settings.  Below is a screenshot of the settings for my drawing template.  Dimensions display as inches because "IPS (inch, pound, second)" is selected, and they're rounded to the nearest 1/16 because I entered 16 in the Fractions column.  You can enter 8, 32, or whatever is appropriate for your drawing.  When I took the screenshot I had clicked on the cell in the More column to show the fly-out.  If you have similar settings, but an occasional dimension displays as decimal instead of fraction, then it's because you don't have "Round to Nearest Fraction" selected.

 

 

If you want your dimensions to show as decimals instead of fractions, then click on the drop-down arrow in the Decimals cell and make the appropriate selection for the number of digits you want to display.  (I almost always choose 4 digits because it bothers me to no end to see 1/16, 5/16, etc. rounded off, but that's just a personal quirk.)

 

 

If on the other hand your drawing is displaying inches and you want millimeters, change the setting to "MMGS (millimeter, gram, second)" at top and choose the appropriate number of decimals you want to show from the Decimals column.  If you want your dimensions rounded to the nearest millimeter you'd select "None" from the drop-down.  If you want something that's not a standard Unit system, such as feet and inches, then select "Custom" and make your selection from the drop-down in the Unit column.

 

By default, even if you have something other than "None" selected in the Decimals column and a dimension is an even millimeter, (inch, etc.),  then the zeros past the decimal point won't show.  If you want them to show, then go to Tools > Options > Document Properties and select "Show" from the drop-down shown below.

 

 

If this change is something you want for future use be sure to save it in your document template (see Why aren't the changes I made at Tools > Options > Document Properties saved when I start a new Part?).

I can't tell you why it's wrong, but I can help you fix it.  Edit the feature and click on the blue arrow at the top of the feature's PropertyManager (it's pretty easy to overlook).

 

 

That will take you to the second page of the PM, where you'll get a preview of the Mirror, and you can select which orientation you want.  Below is the default in the Mirror I used for the example.

 

 

When I clicked on the double caret at right in the box this is what I got.

 

 

If you've mirrored multiple components you may need to click on each one in the Orient Components box and fix each one.

If this is in an Assembly, you likely have a small Part that's a good distance away from the rest of your Assembly.  Click-and-drag a box on the apparently blank space to select anything that's out there, even if you can't see it, then hit the Delete button.  Now try Shift+C again to see if that fixed the problem.  If that doesn't work check your sketches to see if there's a stray sketch element or dimension out there.  If you have a sketch out in space, but have sketches set to Hide, Zoom to Fit will still act like the sketch is visible, and perform accordingly, unless the sketch is set to Hidden in the tree, so you might check that also.

 

These are only a few of the possibilities; there are others.  If the click and drag box and Delete doesn't work, try suppressing components, and any other features, and then try again to track down the problem. Something is almost certainly out there.

 

If it's in a Drawing you may have a small sketch element that's causing the problem.  Try the same method.  If this is a drawing view of an Assembly, with some components hidden, the drawing view outline will still encompass the whole model.  Do a Cropped View around the visible components.  That should fix it.  If you're using SW2015 or later you can use the Zoom to Sheet function instead of Shift+C (SolidWorks Help - Zoom to Sheet), which will ignore the drawing view boundary if it extends past the drawing sheet.

 

On a related issue, I saw a post on the forum from someone that had a feature dimension thrown way away from the model.  It turns out that the problem was caused by an infinite length construction line in the feature sketch.  When the user edited the sketch and removed the infinite length from the construction line the problem went away.  I haven't used infinite length construction lines in years so I haven't personally run into this problem, but wanted to pass it along.  By the way, it isn't necessary to fully define the endpoints of a construction line to have the sketch fully defined, as long as the line's position is fully defined.  That's why I never see a need to have them infinite length (plus it just bugs me to see them extending to the edge of my graphics area).

If you're trying to pattern a feature, such as an Extruded Cut, and not a Body (and no, they aren't the same), and having problems, try selecting "Geometry Pattern" under Options.  If that doesn't help, 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?) .  If, on the other hand you are trying to pattern a body, read on.

 

(In the interest of simplicity, the following discusses Patterns, but the same applies to Mirrors.)  If you're working with a multi-body Part and trying to pattern a single body or combination of bodies, be aware that "Features and Faces" (red arrow below) will be selected by default when you select the feature.  You will get better results if you de-select that box and select Bodies (purple arrow) 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 found that it works much better to create a single feature or body with the sketch, then pattern 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.

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 right, beside the "Mention" link shown above.  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 there's an "Edit" link under "Actions" to the right of your original post you can click on 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.

 

If that's not the case, it's very likely to be a problem with your graphics card.  I am by no stretch of the imagination a hardware expert, but from reading posts here on the forum for years I feel confident in saying that if you have weird graphics issues, and your icon scale is set to 100%, the problem is probably related to 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).

 

At one time I'd have just said to print to pdf instead of saving as pdf, which often produces better results.  That may still be what you need to do, but 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.  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."

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 Employee 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.

This space in the forum is used to document FAQs (Frequently Asked Questions) about the forum itself and the SOLIDWORKS software. Most blogs in the forum are limited to SOLIDWORKS employees posting. But, since Glenn Schroeder took his own initiative to create FAQs using regular discussions, he also has permission and most of the initial content for these FAQs came from Glenn's FAQ posts. Dan Pihlaja has also been added as a FAQ contributor due to his excellent post on using the forum and other helpful posts. Thank you Glenn and Dan for your hard work and dedication to the SOLIDWORKS community!

 

Each FAQ has one or more category assigned to it to aid in browsing and searching the FAQs. On the space homepage (FAQs (Frequently Asked Questions)) there is also listings for:

  • Sticky FAQs which are manually selected/listed by forum moderators. These hopefully make up for the fact that the forums themselves don't have "sticky posts".
  • Popular FAQs which the forum automatically populates based on users visiting the individual FAQs

 

We will continue to look for other ways to creatively use the FAQs in the forum.

 

If you have suggestions for use of FAQs on the forum or the FAQ space itself, post those suggestions in a comment to this post.

If you have suggestions on actual FAQs that should be added, see this blog post: Call for FAQs