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.
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.
First of all:
OK, there is always some confusion on how to vote on SPR's in the Knowledge Base.
(If you don't want to read all of this.....there is a video attached as well)
If things change, I will update this as needed.
9/29/2018: Added "What does voting really do?" area
10/1/2018: "If you are having an issue, and your VAR (Value Added Reseller....the person you [or your employer] likely bought SOLIDWORKS from) can repeat the issue, then they will most likely send the problem to SOLIDWORKS and they will log an SPR (or connect you to an existing one) within the Knowledge Base." was "If you are having an issue, and your VAR (Value Added Reseller....the person you [or your employer] likely bought SOLIDWORKS from) can repeat the issue, then they will most likely log an SPR within the Knowledge Base."
01/02/2019: Updated numbering scheme and added 5Ad
05/06/2019: Updated some pictures representing the latest website updates.
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).
Often, we see many users (both old and new) getting confused about the difference between viewing a thread in their inbox and viewing that thread by opening the thread separately.
Hopefully, this clears up much of that confusion.
To view a thread in your inbox:
After you log in to the Forums, you are directed to: https://forum.solidworks.com/welcome
To view your Inbox, click the little bell icon next to your picture:
This directs you here:
Selecting a thread inside your inbox, shows the thread in a format in which each reply is listed sequentially:
However.....in this format, it is impossible to view attachments, attach files, delete replies or edit replies if you reply to or view the thread from inside this inbox.
The key is to open the thread separately.
To do this, you can do 1 of many different things.
The simplest is to click the thread title:
Alternatively, you can RMB on the title and select Open Link in new Tab or Window (works on both Google Chrome and Internet Explorer).
These work with both Internet Explorer and Google Chrome:
Opening the thread in a new Tab:
CTRL + Click on the link
Click the link with the middle mouse button
SHIFT + Middle mouse click = Open in new Tab and view that Tab.
Opening the thread in a new Window:
SHIFT + Click on the link
Once you have clicked the title and opened the thread separately:
Attachments can now be seen:
And replies are now shown as indented under the message they are replying to (unless the thread has reached a certain length....then indented replies go away and replies are shown sequentially again....but all other things are the same):
And now that the thread is opened separately, access to the advanced editor appears inside a reply.
Also, it is now possible to delete and edit replies. And to branch replies out to a new thread.
See this FAQ by Glenn Schroeder for more information about how to attach files:
07/27/2018: Added Fc and Gc
11/20/2018: Reformatted the numbering Scheme
03/15/2019: added 1Bb screen shot of Deepak's search suggestion
11/08/2019: Updated questions section (2) and discussion sections (3)
01/03/2020: Updated screen shot in Bb
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.
In most cases, sketch entities are shown with a thick line font, but sometimes, you will see some of the entities with a thin line font. The image below shows examples of these thin entities:
In early versions of SOLIDWORKS, all features required the use of a single "contour" (a single loop of connected sketch entities) to be used to create a feature. In current versions of SOLIDWORKS, some features still require single closed contours. Therefore, there are algorithms in the sketcher to highlight cases where the entities do not form a single closed contour since these entities often are created by mistake or will cause problems in downstream features if not corrected. The sketcher tries to display entities that DO NOT form part of a single closed contour in a thinner line font.
Which entities display as thin line font often depends on the entity creation order and also how the entities connect to vertices of the entities that are part of the single closed contour. For example, the first two squares in the image above show different lines in the thin font even though the geometry is the same. This is because of the entity creation order. In the bottom case, the line on the right is shown as thin because it connects to the outer closed contour at a vertex/endpoint. All of the other lines connect to the single contour in the middle of other lines, not at the vertices/endpoints and the algorithm is not designed to highlight these cases.
Depending on the usage of the sketch, the user may not care if there is a single contour in the sketch or not so the thin lines can simply be ignored in these a cases. An example of this is if the user us going to use the contour selection tool to identify which contours will be used for the particular feature.
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.
See this blog post that documents all of the methods to manipulate the view.