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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 

Understanding the difference between sheet formats and drawing templates confuses many new users.  I know it took me a while to get straight.    Sheet formats (slddrt files) and drawing templates (.drwdot files) are two completely different file types.  Sheet formats control sheet size, sheet orientation (landscape or portrait), border lines, table anchor points, and title block notes.  These title block notes are typically driven by model properties or Drawing properties, which can be accessed by going to File > Properties in the Drawing.  You can edit a sheet format by clicking on a blank part of the sheet, the sheet tab, or the sheet name in the tree, and choosing "Edit sheet format" from the drop-down.  (By the way, any existing drawing views and annotations that don't belong to the sheet format will disappear when you go into "Edit sheet format" mode.  Don't worry.  They'll come back.)



When you're finished with your edits you can click on the icon in the upper right corner...



...or right-click again and choose "Edit sheet" from the drop-down to exit the sheet format editing function and return to normal operation. 


You can save your sheet format by going to File and selecting "Save sheet format" from the drop-down.  This will only save notes, lines, etc that belong to the sheet format (stuff that was inserted or edited when in "Edit sheet format" mode).  Drawing views and other notes existing when the sheet format is saved will not be saved with the sheet format.



You can change to a different sheet format by expanding the Scale drop-down in the status bar at the bottom right corner of your monitor and choosing "Sheet Properties..."  (This drop-down hasn't always been available, so if you're using an older version you can right-click again to get the same menu shown in the first screenshot above, but this time choose “Properties…” instead of "Edit sheet format".)



This will take you to the Sheet Properties dialog box (screenshot below), where you can set the sheet scale, change or Reload the sheet format, name the sheet, etc.  When inserting a new sheet, it will use the same sheet format as the active sheet by default.  (If you don't want it to use the same as the active sheet and instead want to choose the sheet format when adding sheets, go to Tools > Options > System Options > Drawings and check the box for “Show sheet format dialog when adding new sheet”.)  If you don't see your saved sheet format listed here, and it's saved at the location you're pointing to at Tools > Options > System Options > File Locations > Sheet Formats, then un-check the box below for "Only show standard format".


Speaking of switching to a different sheet format, starting with SW2017 we can change the format for multiple sheets with one operation.  Choose the new sheet format, then click on the button shown below.



That will bring up the "Sheet Selection" box.  The active sheet will be selected by default, but you can add sheets as needed, or select "Sheet" at the top to select all sheets.



By the way, you might have noticed above in the Sheet Properties dialog box that First or Third projection angle is set there.  I've never understood why.  I'd think that option should be at Tools > Options > Document Properties where it could be set in the drawing template.


Layers are also saved in sheet formats, which I learned by accident.  I had added some Layers to one Drawing that I only needed for that specific project, but after that they'd show up after I'd worked on a new Drawing for a while.  I finally figured out that I had apparently edited and saved my sheet format after creating these Layers, so these Layers would show up when I'd add a new sheet.  I deleted the Layers and re-saved the sheet format.  That fixed it.


As I said above, the title block information is typically driven by custom properties, so if you're constantly opening the sheet format to edit notes I'd strongly suggest you spend some time learning more about custom properties.  In my opinion it's one of the most powerful tools the software has to offer, and will save you a tremendous amount of time, especially if you have Drawings with multiple sheets, since you can enter or edit the information once and it will populate all sheets.  You should only be editing the sheet format to modify other things, such as updating logos, company address, or just the general layout of the title block.  I go months without touching mine.


See the screenshot below.  It's from a newly opened Drawing using my standard template.  I enter the information in the Value / Text Expression column and the notes in the title block are automatically filled out for all sheets.  In the "Sheet 1 of 1" note, both numerals are linked to properties and will update as sheets are added.  The "Draw3" note in the bottom corner is linked to the file location and file name, and will fill in accordingly when the drawing is saved, and the "Scale" note is of course linked to the sheet scale.  As I said above, while I don't, many people also have notes in their title blocks that are linked to properties in the model, and those will update when a drawing view is inserted.



If you aren't familiar with linking Notes to properties, it's as simple as clicking on the "Link to Property" icon in the Note property manager when the Note text box is active, selecting either "Current document" (for Drawing properties) or "Model found here" (for model properties), and then choosing the property from the drop-downs (see below).  If you're trying to link to a model property and don't see the property in the drop-down then insert a drawing view for the note to reference.  You can delete the drawing view later if you want.  (You can link to a property without going to the "Link to Property" icon, in which case I don't believe you'd need a drawing view inserted, but to be honest I've never bothered learning the proper syntax to type in.)



Now for Drawing Templates.  They contain a tremendous number of settings that are controlled at Tools > Options > Document Properties, and can contain a sheet format.  If your drawing template contains a sheet format, but you'd rather have the option to select a sheet format when starting a new drawing, open a new drawing using an existing template, right-click on the sheet format in the tree, and choose "Delete".



Save as "Drawing Template," and in the future when starting a new drawing with this drawing template you'll be immediately prompted to choose a sheet format.


Of course the reverse is also true.  If your drawing template doesn't contain a sheet format and you want it to, you can open a new drawing, choose the appropriate sheet format, and save as drawing template.  Drawing templates are saved by going to “File > Save as” and selecting "Drawing Template" from the drop-down for file type.




Printer settings are also saved in the Drawing Template, so if you have a template that uses a portrait sheet format, but when printing it prints in landscape, open a new drawing with this template, change the printer settings to portrait, and save the drawing template.


Here's a part that throws a lot of people off.  When you start a new drawing it will use the sheet format as it existed when the drawing template was last saved.  The drawing template does not maintain a link to the sheet format file, so if the sheet format is edited in another document it will not automatically update in drawing templates.  If you want your drawing template to reflect changes to a sheet format you can start a new drawing, go to Sheet Properties, and click on the Reload button to update the active sheet.  (I've occasionally run into a situation where the Update button doesn't work.  If that happens, change to another sheet format, click on the "Apply Changes" button, then go back and choose the original format.  That's never failed to work for me.)  If you have multiple sheets saved in your drawing template don't forget to do this for each sheet.  Then re-save the drawing template.  This is why the Layers I talked about above weren't there when I'd start a new Drawing, but would show up when I added sheets.

The information above about new drawings using sheet formats as they existed at the time the sheet was inserted is of course also true for existing drawings.  If you open a drawing that contains a sheet format that has been edited, you will need to Reload the sheet format to update it to the latest saved version.  As I said above, if your Drawing contains multiple sheets, and you're using SW2017 or later, you can update all sheets with one operation.


By the way, I strongly recommend saving all custom document templates, sheet formats, weldment profiles, etc. in a location other than the SolidWorks installation folder so you won't lose them when you upgrade to a new version.  If you're a single user save them somewhere else on your hard drive (and it wouldn't hurt to back them up somewhere else).  If you're in a multi-user environment they should probably be saved on a network so other users can access them, and to help maintain uniformity between users.  Be sure to point to the proper location for each file type at Tools > Options > System Options > File Locations.



2019-06-19 edit:  Added the part about using the icon to exit "Edit sheet format" function.  Thank you Tom Gagnon (Edit sheet format, trapped with no close edit icon ).

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.



Now you can choose the second reference to place the dimension.



This workflow 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 SW2019) 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", with a screenshot of the assignment, 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).  As Kevin Chandler replied to someone that asked for help without showing any effort: "Our enthusiasm is directly proportional to your initiative."


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, and this is work related, the above probably still applies.  We'll be glad to help, but give us some more information, show some effort, etc.  You're getting paid to do the work, not us.

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 value 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.



..or option 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. (Naming dimensions will be a big help if you want to use this option. That will make it much easier to find the one you need.)




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


2020-05-19 edit:  Since posting the above I've run across a situation where neither of the above solutions works.  There's no way (that I can find) to directly reference dimensions in a "Move/Copy Bodies" feature.  The best option I've found is to use something else, like a plane or sketch, to drive the feature.  One example would be when needing to use the "Constraints" portion of the feature to apply a Distance mate.  The alternative would be to create a Plane offset the desired distance, then use a coincident Mate with this Plane instead of a Distance Mate.  The plane value can be linked to a global variable, or configured as needed, which will produce the same result as linking directly in the 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).