5 Replies Latest reply on May 25, 2013 3:24 PM by Andrew Ratsep

    Few drawings/detailing related and other questions

    Andrew Ratsep

      Hello again honoured SW „geeks“. While struggling to have more time with Solidworks I have got another set of questions  You to take a chance with.



      1. I am dealing with already very tired laptop and it happens quite a often that I am forced  to reinstall my operation system. This leads to a case where I also have to reinstall SW software. What „grinds my gears“ most is that I have to customize my SW working environment and preferences all over again...every time.  Well I could probably install software and its additional data to a separate part of the hard disk which will not be deleted even in case of reinstalling the operation system. Let’s say it is potential problem solver. Unfortunately there is never a guarantee that your SW version itself  doesn’t come up with some kind of error or bug. And in that case You are also often forced to reinstall the software and we are back to the same problem. Is there a particular solution to back up your personal preferences or any other suggestion that would help me out?



      2. SW has incorporated a file manager subprogram to manage filing and archiving. To move your files for example to another folder you have right click on the file, select Solidworks, select Move... This is probably necessary not to brake internal references the files have. Unfortunately moving (or renaming) a stack of files with such a  method is painstaking progress. Isn’t there really a way to handle multiple files in one operation...or I am missing something here?



      3. Creating a detail view in 2D environment on the model brings up the corresponding view and its annotation, for example DETAIL A SCALE 1:2. When trying to modify annotation box, the initial text always automatically retains. What’s up with that?



      4. Let’s assume we have a detail with a machined hole in it. The hole is threaded. When trying to section cut only half of the detail then half of the holes thread is revealed. What happens though is that a vertical line referring to thread on the other side shows up as well, as seen on the picture below. Now I had a similar problem  on symmetrical part with holes on both side. Once I section cut one hole, the thread of the other hole shoved up as two vertical lines on the model. Somehow, which I don’t remember anymore, I managed to solve that problem. Is it a bug or what?






      5. Drawing standards allow to present only half of the linear dimension line on half section cuts, when dimensioning diameters, refer to the picture below. Is it possible to achieve this kind of measurement presentation in SW?



      Untitled 2.png

      Much appreciated!

        • Re: Few drawings/detailing related and other questions
          Joseph Weaver

          SolidWorks has a setting wizard which saves all your personal shortcuts, menus, tool bar layouts , etc. After you have your system set up the way you like it, run it and save the file. After fresh install run a restore from it. It's a great tool!

          • Re: Few drawings/detailing related and other questions
            Glenn Schroeder

            1.  Copy Settings Wizard, as explained in posts above.


            2.  Assuming that the files you want to move are all in one assembly or drawing, open the assembly (or drawing), go to File > Pack and Go.  That brings up a dialog box where you can choose a new folder to copy the file to, along with all of it's parts, and sub-assemblies, if any.  At the far left there is a column of boxes that will be checked.  Un-check any of them for files you don't want to copy to the new folder.  There is also a column that says something like "Save to name".  Double-clicking on a file name in this column allows a name change for the new file that will keep the links.  After completing the operation, you can go back and delete the files from the original location, if desired.  This may not be exactly what you wanted, but it's one way to do it.


            3.  I don't know which version of SW you're using.  Starting with SW 2012 you can edit the call-out text for Section Views, and that was made available for Detail Views with SW 2013.  In previous versions that text can't be edited (except of course some settings in Document Properties, which will affect all labels in the drawing).


            4.  Don't know.  Maybe someone else can help.


            5.  You can right click on one of the extension lines and choose "Hide Extension Line" from the drop-down, then right click on the small blue circle at the end of the corresponding arrow head and choose the straight line style.  It will look like the screenshot below.  As far as I know that's about as close as you can get with SW.


            hide arrow and ext. line.png