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FAQs (Frequently Asked Questions)

39 Posts authored by: Glenn Schroeder

A few years ago I started creating plate using the Structural Member function instead of doing it with an Extruded Boss/Base. By doing this the cut list properties for Plate are generated automatically by the software just like they are for Square Tubing, Channel, W-sections, etc., which saves a great deal of time.  The sketch below is an example.



I have a different .sldlfp file for each common thickness, along with a few that I created for a specific project.



The widths are all 2", since it would be impractical to have a separate file for every possible width.  After using the feature I edit the sketch that's absorbed in the feature to match the width I want.  Since weldment sketches are copied when used for Structural Members and not linked you can edit the sketches in the Part without affecting the .sldlfp file.  The Description property is linked to the dimensions, so it will update to match the edit.



Occasionally I want the thickness or width driven by other features in the model, so in those cases I edit the sketch, make the dimension driven, and then use relations to fully define the sketch. (Deleting the dimension instead of making it driven would mess up the property.)


I attached one of my files.  If you like you can modify it to suit, or to use as a template to create other thicknesses.  As I said above, I just edit the sketch in the Part to get the desired width, but if you have a common size you use often I'd recommend making a .sldlfp file specifically for it so you won't need to edit the sketch in the Part.


You could of course create a single file with configurations if you prefer that workflow.


This technique also works well for other non-traditional shapes, like lumber, rebar, wire, etc.

It's a common practice to dismiss an error message and then want it back.  We've probably all been guilty of clicking on "Don't show again" and then dismissing a message without really reading the whole thing, or reading it but not considering all of the ramifications.  Fortunately, getting the message back is a simple process.  Just go to Tools > Options to bring up the Options dialog box.  Go to the System Options tab (it should be open by default), go to "Messages/Errors/Warnings", and check the appropriate box (or boxes) for the message(s) you'd like to bring back.



By the way, while I'm on the subject of these messages, while there are some that I think should have the "Don't ask again" option and don't, the "Confirm Delete" is one I don't think should have that option.  Whether or not to delete child features and absorbed features when deleting a component from an Assembly, or whether or not to delete the sketch when deleting a Section View or Detail View from a Drawing, or if you want to delete a sketch along with a feature in a Part are just a few examples.  I had that one deleted for a while, but never again.

   There isn't a way to do that directly.  You have several options.


  1.   Click on the sketch in the tree and Ctrl+C to copy it, and then open the Part file, select a plane or face (assuming it's a 2d sketch), and Ctrl+V to paste it.  The internal dimensions and relations will stay with the new sketch, but any relations or dimensions to elements outside this Part won't carry over, so you'll need to edit the sketch and add relations or dimensions as needed to fully define it in the Part.  If you're editing the Part within the Assembly you can reference other components.  After closing the new sketch you can delete the original sketch in the Assembly.
  2. Edit the Part within the Assembly, create a new sketch on the same plane or face 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.
  3. Just chalk it up to experience, delete the sketch in the Assembly, and re-create it in the Part.  It's good practice, and it should go faster the second time.


2019-08-30 Edit:  See the replies below from Justin Pires and Dan Pihlaja for even more options.

   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.  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 (it 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 you can still click on the box at the end of the extension line and re-attach it.

     (2019-08-22 Edit:  If you created the dimension by right-clicking on an edge and choosing "Select Midpoint" from the drop-down, I've never found a way to re-attach it.  If you know of one please share 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.



2019-11-04 Edit:  That default color for lost references can be overlooked, so I changed mine.  It's much less likely to be overlooked now.


If you have multiple configurations in your model, and edit a dimension that's shared by all configurations, by default that change will affect all configurations. I personally like it that way. If I haven't told the software that this dimension should differ between configurations then I want any changes to affect all of them. Others may disagree. Now that I have that out of the way, there are several ways to edit a value only for selected configurations.


1. One way is to open the standard dimension dialog box for the value, click on the Configuration icon, and make the appropriate choice. If you do this outside of an active sketch then you'll probably need a manual rebuild for the change to take affect.



2. Many people use that method, but I prefer another workflow that doesn't require me to be in "Edit sketch" or "Edit feature" mode. In fact, it only works when there isn't a feature or sketch active. I single-click on the feature or sketch in the tree to display the values. (If you don't have Instant 3d turned on then you'll need to double-click on the feature, or go to Annotations at the top of the tree and choose "Show feature dimensions".) I then right-click on the dimension in the graphics area and choose "Configure Dimension" from the drop-down.



This will open up a simplified design table, with a column for the configuration names and one for the selected value, and a row for each configuration. You can enter the desired value in the appropriate cell for each configuration in this table.



While this table is open you can double-click on other dimensions, sketches, or features to add columns. If you double-click on a sketch there will be a drop-down where you can select sketch dimensions to add.


As you can see at the bottom, you can also create new configurations from this table. I often use this method to create new configurations instead of going to the configurations tab and adding them there.


If you'll enter a name for the table at the bottom you can save it for future edits, but the changes you make in this table will still be saved even if you don't save the table. And as I said above, after closing this table you've effectively "told" SW that this dimension is configuration specific, so if you want to edit the dimension later you don't need to re-open the table. You can just click on the feature to show the value in the graphics area again, click on it, and change it to the new value. That change will only affect the active configuration, and won't require a rebuild for it to take effect.



2019-03-07 edit: My wife and I (mostly her) are having some remodeling done, and because of that the TV is unhooked, so I'm sitting at my laptop browsing through some of these blog posts, and it occurred to me that I should give some credit. I learned about this option from Paul Marsman at question about linear patterns and configurations.


3. A third method is to set up an Excel-based design table by going to Insert > Tables > Design Table. That will open a property manager where you'll have a number of options. Below is the result for this Part when I chose the default settings, including "Auto-create". As you can see, it adds a column for every dimension and custom property (I highlighted the column for the same dimension I used in the methods above). If you don't need or want that many columns you can choose "Blank" instead of "Auto-create" and only add the parameters you want, or of course delete columns from the auto-created table.



I don't use the Excel-based design tables much, so if you have a specific question about them I'd encourage you to post the question in the forum instead of in a Reply here, and I'm sure someone will be glad to help. By the way, I know people follow the forum from several different places, but I generally do it from the All Content page. It's very simple to start a new Discussion from there.


Open and run the attached .exe file first posted by Kevin Chandler at Find lost dialog/window utility (using Autohotkey) V1.01 update (posted again by Tony Tieuli in a Reply at Drawing Rotate View dialogue box doesn't appear: any ideas on getting it back?).  It will bring it to the front.


Edit:  An alternative is to use the method described in the Reply below from Dan Pihlaja (thank you for posting that Dan; I thought I remembered seeing something somewhere about a method using the keyboard, but couldn't find it).

If the only variable will be the visibility of components I recommend hiding them with display states instead of suppressing them with configurations.  While it may not always be the case, using display states will usually result in a smaller file size, but to me that's a secondary reason.  If other components are mated to a suppressed component then those mates will be suppressed, which can obviously cause problems.  The mates will remain in effect when a component is hidden in a display state.   If there are any disadvantages to using display states I'm not aware of them.


Edit:  Just because I wasn't aware of any disadvantages to using display states instead of configurations doesn't mean there aren't any.  Please see the comments below.  I mainly use display states to hide selected components that I don't want to show in a drawing view, so it's typically done after the Assembly is finished, but as Paul Risley  said in the second paragraph, using display states as a design evolves can cause issues (although, the checkbox for "Hide new components when inactive" in the display state Properties will help with that), and I'll agree with him that configurations are easier to edit.  And as Dan Pihlaja  said, mixing configurations and display states can certainly get confusing.  Configurations by themselves can get confusing, as far as that goes, especially if there are multiple layers of Assemblies.


It boils down to you taking the information here, both above and below, and choosing the best option for your situation.

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.


To start off, if you received an Assembly from someone else without the Parts and/or sub-assemblies, there's nothing you can do.  You can't open the Assembly without those files.  Ask the person who sent it to you to do a Pack and Go of the Assembly to a zip file and send that to you.  If you aren't familiar with Pack and Go, see How can I create a new Assembly or Drawing similar to an existing one?.  If they don't know you need the Part files to open an Assembly it's very likely they never heard of Pack and Go either, so you might send them that link also.


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



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



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


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



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



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

Like most things in SolidWorks, there are several ways this can be done.  Probably the simplest starts with orienting the model the way you want the drawing view to be.  That can be done a variety of ways.


Two of the simplest are starting with one of the standard views and rotating by holding down Ctrl and using the right and left arrow keys on your keyboard, or by Ctrl+selecting two non-parallel surfaces and then the Normal to button from the Standard Views toolbar, which will place the model with the first face selected normal to your screen and the second surface selected at top.  (See this blog post from Jim Wilkinson for more ways to manipulate a model.)  When you have the model oriented the way you want, hit your spacebar.  That will bring up the Orientation dialog box.  Select the New View icon.



Name your view and save, and the View will be available to use in your Drawing.  Select it from the view's PropertyManager.



If your drawing view has the correct face normal to the screen, but you need to rotate it, you don't need to create a new view.  Just click on the drawing view to highlight it, then click on the Rotate View icon in your heads-up toolbar (see below).  That will allow you to enter a value for how much you want to rotate it.  It will rotate counter-clockwise, so if you want it rotated 90° clockwise you'll need to enter -90°.  By the way, I occasionally have a body that comes into the drawing at an odd angle because that's how it's oriented in the model.  When that happens, and I want it horizontal or vertical, I place a sketched line in the view, make it horizontal or vertical, then use the Smart Dimension or Measure tool to determine the angle between it and a model edge.  That's a big help with knowing what value to enter for Rotating the view.  Delete the line and dimension after determining the value.



Another option for rotating a view is to select an edge of a drawing view, go to Tools > Align Drawing View, and select "Horizontal Edge", "Vertical Edge", etc., but you may or may not get the results you want.


Still another option is to 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.  If this is a multi-body part 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.  This might be a good option if you're in a multiple user environment, because if someone updates the model's standard views it won't affect drawing views that were inserted using this method.


Relative View was one method commonly used for showing selected bodies before the Select Bodies... button was added (see How can I show a single body of a multi-body Part in a Drawing?), but I don't believe I've used this method since then.  Once you've clicked Okay you can't go back and edit your selections, which is one big reason I don't like to use it.  I described it here because it's an option for a drawing view orientation without the need to create a new view in the Part file.


2021-01-07 Edit:  I just learned about a new way from Betty Baker.  In the Drawing, go to View > Modify > 3D Drawing View.



A dialog box will pop up in your Property Manager asking you to select a view.  After doing so you'll get the toolbar shown below, and a blue box will appear around the drawing view you selected.  Now you can use one of the icons to manipulate your view, or click and drag directly on the view to rotate it in 3 dimensions.  After doing so you can Save the view just like described above when creating a custom view in the model.


Of course if you have a backup try opening it.  If you don't then try opening the file with a different method.  I typically open files by selecting them from Windows Explorer, but when getting that error I can usually open the file by going to File > Open and browsing to and selecting the file that way.  You might also try just clicking on the file in Windows Explorer and dragging it into the SolidWorks window.



If none of that works, right-click on the file in Windows Explorer and choose "SOLIDWORKS > Pack and Go..." (assuming you have SolidWorks Explorer installed).  That will open up the Pack and Go dialog box.  Save the file to a different location and try to open this new one.  If it opens okay you can save it over the original, or just continue working with it in the new location.



If this still doesn't work, you may have to send it to your VAR to see if they can help, or you could try posting it on the forum in a new Discussion (please don't do it here) to see if someone else can open it, save it, and send it back.

As a disclaimer, I don't pretend to be any kind of hardware expert, so the information I give here will be mostly a compilation of stuff I've picked up reading posts on the forum.  Now that I have that out of the way, the answer to what kind of computer you need will depend on your specific use.  If you do a lot of rendering I understand that can affect the answer.  For most operations SW uses a single core, although I believe that might not be the case for simulation (see the Reply from Nick Birkett-Smith  at New Computer for Solidworks question: 1 Processor with 12 Core or 2 processors with 4 core each), so if you're just doing basic modeling and Drawings you won't get much benefit from multiple cores.  What IS the Best CPU for SOLIDWORKS?  and  are other sites you might want to check out.


Don't get a gaming video card.  While some people use them without major problems, many aren't that lucky, and I seem to see a lot of posts from people who were using one and an automatic driver update made them completely unusable for Solidworks.  Get a video card (and driver for it) that's recommended by Solidworks.


When you get a preliminary selection, go to this site to evaluate it, and then I'd encourage you to contact your VAR (Value Added Reseller; the company you bought Solidworks from) and get their input.  Be sure to tell them what kind of work you'll be doing.  I'm pretty sure they'd rather help you select a machine that works well now instead of getting calls asking for help when you get a bad one.


If you're a student, or off subscription, and therefore can't ask a VAR, the site I posted above should help, or do a search in the Discussion section of this forum (Boxx Apexx OR Dell Precision? posted by Rob Edwards would be a good place to start, or Buying New CAD Workstations  or Computer for Solidworks 2018, or do a search for posts by Charles Culp, who has given some excellent advice to many people, including me, although he hasn't been around the forum much lately).  If a search doesn't help feel free to post your specs there in a new Discussion.   I'm sure someone will be glad to give you some input.


I'm not going to recommend any specific brands, but while I've always used Dell, and have had good luck with them, I've heard many good things about Boxx (Custom Workstations for Your High Performance Computing Needs | BOXX) and SolidBox (  It's my understanding that they will optimize a computer for use with Solidworks.  If I was buying my own instead of my employer providing it I'd probably look into getting one from one of those companies.


If you're thinking about a Mac I'd encourage you to reconsider.  If you really want one (or already have one), and only need SolidWorks for a class or occasional use, see  2019-20 Student Edition on a Mac, and maybe the post from Anna Wood at what is the best way to run SW on a Mac laptop?.


I'm attaching the specs for my computer.  Again, I'm not advocating for any brand, but this one works well for me (and I did have the helpful people at GoEngineer review the specs for me before getting it).  I work with Parts, Assemblies, and Drawings, but I don't do any Simulation or Rendering, so I can't promise a similar machine will work well for you.  (2020-04-19 edit:  I'm attaching the specs for my new computer, but I'll leave the previous one. So far the new one is working well also.)


Edit:  I saw the information below posted by Mathieu Myrand-Bolduc in a Reply on the Discussion section of this forum, and he graciously agreed to let me quote it here.  There's some good stuff in it.


"The place I work at does a lot of things through the API, some of it takes a lot of time, up to several hours actually, so we looked into a lot into the performance question, plus like @Jeff Mowry I like to game, so we went for what amounts to a high power gaming rig with a Quadro/Firepro video card.  But in the process, we learned a lot about how Solidworks uses the hardware.  The following is a resume of what we discovered.  It was evaluated on SW 2016 and we mostly evaluated Intel/NVIDIA hardware.  The conclusions "should" hold true for AMD hardware.  Please note that we are running 3K components + sheet metal assemblies, so this should be a rather high end machine.



Assembly/rebuilds/Part creation: Uses a single core.  If what you mostly do is Part and assembly creation, go for a High clock speed cpu.  Note that more recent are usually a bit more powerful (a few % points).  We went for a intel I-7 6700K.  Theoretically you could go for a I-5 if you wanted to save some money, since the major difference is the hyper-threading and you have other cores that are free, so it shouldn't slow you down too much. Xeon were not evaluated, since the cost for high speed cpu was ridiculous and we didn't feel their differences added anything to us.  Besides we had enough of our 2 core 2.5 ghz machines .....


Drawings: This is a bit different, since the view regeneration uses multiple cores.  If you don't have to rebuild the assemblies, then go for a bigger core count.  You want a high clock speed too for the odd time when you must rebuild.  We didn't test this specifically, but that's what came up on several resources .


Rendering, FEA: We didn't test, but unless Solidworks did something weird these operations should be able to use multiple cores, so my guess would be a high core count.  I would guess the new I-9 would shine there.



All operations: As much as needed.  If you are working with small to medium assemblies and not opening anything ram heavy, then 16 gb should be enough.  We went for 32 gb thought and I personally saw solidworks eat 22 gb on a single assembly (yes I opened it in resolved mode ....).  Most recent high end cpu can go up to 64 gb, maybe 128 gb (probably an overkill).  I have seen a benchmark suggesting that ram speed does not matter much on gaming performance, so I wouldn't worry about that too much.



Get a pro card, Quadro/Firepro.  You can use a gaming card, but you loose a lot of performance and get weird results.  I tested this at home (I have a Geforce 970) and It was a lot slower and less stable than what I had at work.  I will admit that I didn't test without the registry key hack to enable real view and the other advanced options.  I noted that the shaded with edge option was particularly slow on my machine.  I suspect that there is special hardware in the Quadro/Firepro gpus.  We have mid range Quadros and it works fine for medium/big assemblies.  It is used mostly when you play with the views (rotation, move, display state changes , etc...).


Hard disk:

As fast as possible.  This affects everything, from boot time to opening Solidworks to opening and saving of files (on the hard disk of course).  I would recommend the new M.2 hard disks, check the benchmarks, some are truly better.  We have Samsung EVO 850, but the new ones are a lot faster.


Final notes on overclocking the CPU.  CPU clock speed and performance are just about linear, so double the speed and you should just about cut the time in half.  However, unless you spend a LOT of time in an intensive CPU operation, the gains in a day won't be that impressive for a user.  Especially since you won't do more than a 30% clock speed increase (we did 15% I think).  If you buy an OC box, sure, they tested it and are giving you a warranty on it, but if you want to do it yourself, unless it's for fun, I would leave it stock (or maybe boost all cores to turbo speed), or be ready to spend some time testing stability.  We did it, because we are doing CPU intensive stuff, but you have to be careful, Solidworks can become unstable even if your system looks rock steady."

2020-02-25 Edit:  You might also like to review Hardware Certification from Jeremy RIEDEL

In the simple example shown below, I'll edit the green part to add a hole that will be linked to the hole in the red part.



First I'll click on the green part (either in the graphics area, or in the tree), and choose the "Edit Part" icon.  You could also choose "Edit Component" from the Assembly tab of the Command Manager.



The text for the selected Part will turn blue instead of black in the Feature Manager tree.  You are now free to edit the Part within the Assembly just like you would in the Part file, and you can reference features from other Parts just like you would if they belonged to the Part being edited.  Select the "Edit Component" icon in the Command Manager to exit the "Edit Part" function when you're done.



Now the green part references the red part, and any edits to the red part will be reflected in the green one.



As you can see, the hole was near the top of the blocks but is at the center in the last screenshot.  I edited the hole in the red part, and the hole in the green part updated without any input from me.

Insert the drawing view and insert the Bill of Materials (BOM), like usual, but after inserting the BOM you can delete the drawing view.  After it's inserted in the drawing the BOM is linked to the assembly file itself, not the drawing view, and will still update if the assembly is edited, even if the drawing view has been deleted.  If you don't want to delete the view for some reason, you can move it off the sheet, or Hide it.


Because of this behavior, if you have inserted a drawing view of an assembly and a BOM, and then change the drawing view to show a different configuration, the BOM will not automatically update to reflect this configuration.  You can go to the BOM's Property Manager and change which assembly configuration it's referencing.  In the example shown below the Assembly only had one configuration, but if you have more you can choose which one you want the BOM to reference.



If you want to keep the drawing view visible and in it's present location, but the BOM won't fit on the same sheet, you can move it to another sheet.  Go to your tree, find the BOM, click on it, and drag and drop it on the sheet name of the sheet you want it moved to.  You may need to rebuild for the move to take effect.


With the parent file open, go to File > Pack and Go.



This 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).


There's more information at 2019 SOLIDWORKS Help - Pack and Go Overview