Common Support Calls in November '11
Welcome to the third edition of this, the Innova Systems Technical Support Newsletter. Our Technical Support team have been working hard, compiling some tips and tricks to handle some of our more common support queries. If you missed last month's, catch up here.
Applications Engineer, David Durston shares answers to ten of this month's most common support calls with an additional tip from Matthew Fordham - our resident SolidWorks Simulation expert...
- Belts and chains - how to add in sketches, and assemblies
- How to cut one part with another
- Where have linked values gone?
- How to specify local working folder in Workgroup PDM
- Is "MOD-DIAM" showing instead of diameter symbol in dimensions?
- How do I change a radius dimension to a diameter?
- Upgrading your toolbox installation - Best practices
- Choosing which drawing populates the view palette
- Work out total length of same profile cut list items
- Configure Mate references
- Simulation Tip - Average results across boundary for parts
1. Belts and chains - how to add in sketches, and assemblies
If you have pulley parts in an assembly or if you have a sketch with circles in it you can use SolidWorks to automatically create your belt components.
- For assemblies select Belt/Chain from under the assembly features menu.
- For sketches you can find belt/Chain under tools/Sketch entities.
You then select what you want the belt to go around and which way and let SolidWorks take care of the rest!
2. How to cut one part with another
If you want to cut one part out of another part then you can use the indent command. This command requires two intersecting bodies. You then select the body you want to indent and the tool body (the body doing the indenting). The cut option just removes material representing the tool body, otherwise the shape of the tool body will push through to the other side of target body. You are also able to set a clearance value between the actual size of the tool body and the indented shape.
3. Where have linked values gone?
One of the changes in 2012 is the equation editor. Alongside this the link values command has been removed. This won't remove your existing linked values and you'll still be able to edit them but the method for creating the new equivalent is slightly different.
When you start to dimension your entities, for the first one type '=MyGlobalValue' (where MyGlobalValue is the name you want to use) You will be asked if you want to create a new global variable, which you do!
You will then be put back in the dimension box in order to give your new global variable a value (you can tell this because of the globe at the front of the dim box). The dimension will then show the equation symbol. In each additional dimension that you want to equal this value merely type the equals sign and then from the drop down menu that appears highlight 'global variables' and select your global variable from the list.
4. How to specify local working folder in Workgroup PDM
In order to specify which folder files checked out of the PDM Workgroup vault will be saved into, right click in the vault area of the task pane and choose options.
On the tab 'Folders' fill in the box with your preferred folder. Files you check out will now by default check out into this folder enabling you to find and manage them more effectively.
5. Is "MOD-DIAM" showing instead of diameter symbol in dimensions?
When you add a diameter dimension to a drawing and get "MOD-DIAM" instead of the diameter symbol, and this persists after a restart of SolidWorks, then unfortunately your gtol.sym file is corrupt. This can be fixed by running a repair of the SolidWorks installation with the installation manager via the windows control panel or by copying the file from a working installation and replacing your corrupt version.
The file 'gtol.sym' can be found here:
C:\Program Files\SolidWorks Corp 2012\SolidWorks\lang\english\
Just rename your version and paste in the copy.
6. How do I change a radius dimension to a diameter?
If you have put a radius dimension down in your sketch and then want to change this to a diameter dimension you do not have to delete the dimension and then re-add it. Select the dimension and in the properties manager click on the leaders tab. This will show you several icons. If you click on the 2 icons indicated you can now alternate this dimension between a radius and a diameter. Or alternatively right click on the dimension and select “display as...” (or in drawings, right click and select “display options”).
7. Upgrading your toolbox installation - Best practices
If you have spent time adding custom information to your toolbox then you don't want to lose this when upgrading SolidWorks, also if you use the toolbox a lot then it already contains many created (used) configurations. Or if you have multiple toolbox locations when you upgrade SolidWorks they may not all update to the latest version.
In all three cases you may get the warning 'toolbox database is not the expected version'. To stop this error message you need to use the manual toolbox updater.
- The program 'Updatebrowserdata.exe' can be found in C:\Program files\SolidWorks Corp\SolidWorks\Toolbox\Data Utilities\
- Run this program and you will get a window that looks like this:
- Ensure the database to update box is correctly filled in and that there are numbers next to both database version and update version. Then click Update and you are done.
8. Choosing which drawing populates the view palette
On many occasions you want to have drawing views from more than one model file in a drawing. If this is the case then you can populate the view palette with the drawing views of any model file by selecting the file in the drop down box at the top of the view palette if it is already open or by browsing for it by clicking on the 3 dots ( ... ). Once you have selected your file click refresh and the view palette will have available views for this file.
9. Work out total length of same profile cut list items
Sometimes you need to see total length rather than the number of each weldment item if so then you can use a bill of materials.
- Generate a BOM (not a cut list!) and set to indented
- Un-tick detailed cut list
- The BOM will show the type of profile and then the total length for that profile
If you have created a mate reference on a part, and then generate lots of configurations of that part, you may find that the mate reference automatically suppresses in the newly generated configurations.
Configure mate reference is not available on the right mouse button like it is with features and dimensions. In order to configure your mate reference. Righ click the mate reference and select properties
Within here you have a configuration drop down menu which allows you to configure whether it is suppressed or active in the various configurations.
11. Simulation Tip - Average results across boundary for parts
One commonly overlooked results option is the 'Average results across boundary for parts' tick box. You can find this option if you edit the definition of any of your stress results plots and expand the 'Advanced options' settings box in the feature manager window. As you will expect from the name, this option will plot the average stress value across two coincident faces of different parts on both of the faces in question. In some (not all) cases, this will cause erroneous results where the average of two opposing directional stress values cancel each other out and can conceal their existence.
