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   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.

 

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:

  1. If any of this information is incorrect or inaccurate, please add a comment below and I will look into fixing it.
  2. If you think I should add anything else here, or I am missing a step....comment below.

 

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)

 

  1. Wait....what is an SPR?
    1. SPR stands for Software Performance Report and is the method that SOLIDWORKS uses to track bugs and enhancements.
    2. If you are having an issue, and your VAR 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.
    3. VAR stands for Value Added Reseller....the person you [or your employer] likely bought SOLIDWORKS from
  2. OK....but how do I access the Knowledge Base?
    1. Well, you head over to customerportal.solidworks.com
    2. This will bring you to:
    3. Logging in will bring you here:
    4. If you have a VAR, this screen will tell you who it is and how to contact them (in the bottom right corner). Mine is listed there. Yours might be different.
    5. Now, at this point, you will want to click on the "Knowledge Base" link:
    6. This will bring you here:
  3. Ok, I have accessed the Knowledge Base.....how do I find the SPR I want?
    1. Now, you have a choice.
      1. If you know the SPR number:
        1. It should be a 6 or 7 digit number without letters, then simply type it into the search bar and hit enter. Example below:
        2. Selecting that SPR brings me here:
      2. If you don't know the SPR number:
        1. Then you can search for keywords in the search bar.
        2. Some tips for searching:
        3. If you put a phrase in "quotes", then it will search for exactly that phrase.
        4. If you have a phrase and you don't put in quotes, then your search will result in all SPR's with any of those words
        5. I have found that sometimes it is easier to figure out the correct terminology by using the SOLIDWORKS help, then coming back here to search for it.
        6. You can refine your search results using the menus on the left.
        7. Example:
  4. OK, I have selected my SPR....now how do I vote on it?
    1. OK, voting really isn't intuitive....but here is how you do it:
      1. Once you are in the screen showing the SPR:
  5. What does voting really do?
    1. Voting on an SPR does these things:
      1. If the SPR changes or is fixed, you will get a notification regarding this.
      2. It lets SOLIDWORKS know that there is more interest in this particular issue.
      3. This is why it is really important to get your VAR involved when you have an issue so that the issue can be tracked via the SPR channel.
      4. I have been told that 60% of all the SPR's out there only have one vote attached to them. Simply adding a 2nd vote to one will float it to the top (so to speak).
  6. Conclusion
    1. There you have it.
    2. Voting on an SPR isn't really hard to do....it is just not intuitive.....so I think that it scares a lot of people away.
    3. Maybe this Blog post will help ease some of that confusion/fear.

 

If things change, I will update this as needed.

Change log:

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).

Other options:

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:

How can I attach a file to a forum post?

  1. If you are new here....please look into these threads.
    1. Get Started in the community
      1. Tips on how to create your profile and stay connected (to say the least!)
    2. Forum Posting
      1. Tips on searching for answers, posting a question, updating your profile and editing posts (there's more too!)
      2. Here is a screen shot of one of the most important steps from the post:
      3. Written by Deepak Gupta
    3. Request for Forum Etiquette
      1. A general reminder of etiquette while on a public forum and where to post off topic responses.
      2. Written by Dennis Dohogne
    4. Please use the Quote Previous Message Functionality
      1. Tips on how to quote someone else while replying to a post (very important, especially on long threads).
      2. Written by Jim Wilkinson
    5. How to ask a good question in the API forum
      1. This one is specific to API, but I think that it applies everywhere else, too!
      2. Tips on how to keep questions short and to the point
      3. Written by Keith Rice
  2. Regarding Questions:
    1. First, please do some research. Either by searching using the tips from Forum Posting or by searching using these Excel documents that John Stoltzfus has created.
    2. If you've asked a question and have received a sufficient answer to move forward, then please MARK THAT ANSWER AS CORRECT.
      1. If there are multiple answers that are correct:
        1. Then post a reply summarizing all the correct answers (make sure you give them credit) or
        2. Pick the best suited one.
        3. If multiple answer are the same, then pick the one that was posted first.
      2. This is important for future people who are trying to find the answers to their questions
        1. The ones who are following the tips listed above in the linked posts.
    3. If you found the answer on your own, then please post the answer for other people who have the same question.
    4. If you have not received a sufficient answer, please don't post the question a 2nd time. Other options include:
      1. Edit the question and reword it or add pictures and attach models.....maybe no one understands.
      2. Post a "bump" reply to your own question.
        1. This will pop it to the top of the forum page. (or just edit it and hit post without actually changing anything)
    5. If you post a question, and later, have a different question:
      1. Please create a new question instead of asking the question in your original one.
      2. This is important, because the new question can easily get lost in the hustle and bustle if just posted as a reply.
    6. When you ask a question, please reference which version of Solidworks you are using. This will help a lot.
    7. Posting screen shots with your question will help the answerers a lot as well.
      1. The Windows Snipping tool comes with Windows 7 & 10 for free. Link for instructions on how to use snipping tool.
      2. I personally use Greenshot, a free program for capturing screenshots. http://getgreenshot.org/
      3. Once you copy the snapshot, you can just paste it right into the body of your question.
    8. Uploading a file generally helps a lot.
      1. If you can't share the actual file, then recreate the problem in a sample file and upload that.
      2. Use Pack and Go to create a zip and upload that. 2017 SOLIDWORKS Help - Pack and Go Overview
      3. How can I attach a file to a forum post? written by Glenn Schroeder

  3. If you don't actually have a question, but you still want to discuss something that you feel is important:
    1. Then you can uncheck the "Mark this discussion as a question" check box.
      1. This will turn this thread into a discussion rather than question and open the floor up for lively discussion.
  4. If you have created a question and someone has a secondary question, or the topic has gone in a different direction:
    1. Then as the author of the original question, you have the option to "Branch" a discussion out into a separate thread.
      1. This is also important for future people who are trying to find the answers to their questions

 

 

Edit History:

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

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:

ThinSketchLines.png

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.

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.

See this blog post that documents all of the methods to manipulate the view.

How do I manipulate my model view; let me count the ways

Most options about your forum profile can be changes using theEdit Profile page within the forums. However, your name and e-mail address actually come from your SOLIDWORKS ID which is defined in and used by the SOLIDWORKS Customer Portal and must be changed there. To change your name or e-mail address do the following:

  1. Go to www.solidworks.com
  2. Click the image of the avatar in the upper right and then the link to the SW Customer Portal and enter your login if prompted:
    login.png
  3. Choose the My Profile link in the quick links on the left:
    profile.png
  4. Choose the "click here" link shown below the My Profile section indicated that you want to request a change to your email address or company information.
    clickhere.png
  5. Make the desired changes in the form that comes up and hit Submit.

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.