When you install Solid Edge, a number of template files are installed into the C:/Program Files/Solid Edge ST7/Template folders (split into sub-folders to define the drawing standards). Each folder will contain five files that cover the five different environments – Part, Sheet Metal, Assembly, Weldment and Draft. These files hold the pre-configured layout and styles associated with the drawing standards, including units, projection, dimension styles, line styles, etc.
When you create a new document, you will select an environment and Solid Edge will open the file for you. What is does in the background is to copy the template and create a temporary file of the template. Most of you will have created your own template draft file, applying your own drawing border and then saving this into the template folder of your preferred drawing standard. If you work in sheet metal, you may do the same by setting up multiple templates that have pre-configured material, thickness, bend radius and gage settings, so that you can start designing immediately without having to go through setting all of these up each time.
In Solid Edge, styles govern the stored format of an item, whether it be a line, face style (colour) or dimension. These styles are stored in a template document, with many standard styles delivered in the templates documents. Styles cover all of the standard element types (and will vary in different environments) and will have different settings, depending on the style type.
To create a new style type, click on the Styles icon in the dimension section of the Home tab.
This will open the Style dialog box. The first step is to find a style that is similar to the one you want to create, so click on the style type and style closest to what you are after.
One style I like to create is for a radial dimension so that the text is displayed horizontally rather than parallel to the dimension line. In this example, click the dimension style type and the ISO (mm) style and then click the “New” button. On the Name tab, enter “ISO Radius” in the name box as a label for the dimension style.
Next, click on the Text tab and change the Orientation from Parallel to Horizontal. Click OK to save the new styleand this will now display in the dimension style list. Close the style disalog box.
When you dimension a radius/diameter, the standard ISO format is to display the dimension parallel to the dimension line, but now that the new style has been added, when can change the style from the Dimension options bar and change to our new style to give a different display to the placed dimension.
As explained earlier, these styles are stored in the file you are working on, so if you add it into one drawing, it will not be available in another that was created earlier. Ideally, your own styles will be added into the template document before they are used, so that these styles will be available in all files created. This, however, is not always possible, so to copy styles from one file to another, we need to use the style organizer.
The Style organizer is accessed from within the styles dialog box and allows you to copy a style to/from an external file to Solid Edge (Materials.mtl) and the current file.
When you open the Organizer, the dialog box will display the styles that are held in both the materials.mtl and the current file. Select the style that you want to copy and click the copy button to copy it into the Materials.mtl file.
When you open your other file, open the Styles dialog box and then the Organizer. Select the style from the list under the Materials.mtl and the select the Copy button to copy it into your existing file.
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