Splitting Views of a Drawing
Most users are aware that a Solidworks Part window can be split into 2 or 4 panes by using the standard Windows splitter-bars. But this capability is not available in the Drawing environment. What is the best way of performing tasks that require close-up zoom in two different areas of a drawing? For example, cutting and pasting a body of notes to a different corner.
Use the command Window – New Window.This creates a complete duplicate of the Drawing’s document window, including FeatureManager. Then choose Window – Tile Horizontally (or Tile Vertically). You can now pan, zoom, and create or edit geometry in either window independently of each other, but both windows portray and update the same drawing file.
Note: In SolidWorks 2007 or later, you can hide the FeatureManager in one or both of the document windows for easier viewing.
Attaching Datums to a Dimension
Some company drafting practices permit attaching a datum call-out directly to a dimension. For example, if the centerline of a diameter is to be the -A- datum, the datum symbol could appear directly below the diameter dimension, instead of attached to the centerline. This doesn’t seem possible at first, because Datum symbols in Solidworks will not ‘dock’ onto a dimension, only onto a model edge.
The solution is to create a Geometric Tolerance, with all fields empty except the 1st datum reference, where you type “-A-”. This symbol can be dragged onto a dimension, docking onto it. The Geometric Tolerance control frame will look exactly like a Datum call-out.
SolidWorks 2007 adds the ability to directly attach Datum Symbols to dimensions and geometric tolerance frames via drag-and-drop.
How do I Create Notes with Multiple Leader Lines?
This is one of those functionalities in SolidWorks that is hiding in plain sight. There are no pull-down menus or dialog check-boxes to do this, because it uses the Windows Control-drag method.
First, click on the note to select it. When it highlights, you will see a square, green drag-handle at the end of the leader arrow. Place your cursor directly over this drag handle, hold down the Ctrl key, and drag-and-drop a copy of the leader to a new location. Repeat if you want more than two leaders.
What Affects eDrawing Size?
There are several factors including display options, file type, and model complexity. An eDrawing is a special format developed by SolidWorks to compress and view a drawing file with additional 2D/3D hybrid viewing and animation. The format has been optimized for small file size to ease distribution of model data via the internet or portable disk. There are a few choices you can make to make these compact files even smaller.
First, there are a few different file types to save eDrawings as. You can save just the eDrawing itself (*.EDRW), or you can save a self-extracting, self-viewing type (*.EXE), or you can Zip up the EXE file to help it through firewalls (*.ZIP), or you can send an HTML version of the eDrawing (*.HTM).
If the recipient has the eDrawings Viewer installed (available free from www.edrawingsviewer.com), then you only need to send the EDRW file. Otherwise, any person running Windows can run the EXE to open and manipulate the eDrawing. The EXE has a viewer embedded in the file, along with the CAD data, which adds about 2 MB to the file size. The ZIP file is generally the same size as the EXE file would be. The HTM file is only a couple KB larger than the EDRW file and will open in Internet Explorer, thus helping the recipient to download the required eDrawings Viewer if he or she does not have it installed.
Another factor that can affect eDrawing size is the image quality of the 3D model. As described in another tech tip, the setting for Tools – Options – Document Properties – Image Quality – Shaded resolution affects SolidWorks part and assembly file size (if saved in shaded mode), due to the number of graphical facets. This is also true of eDrawings. When an eDrawing is published, the settings of the SolidWorks models are used to determine the quality of the 3D image. Higher shaded image quality leads to larger files. For example, a test run publishing an eDrawing of a 1″ diameter sphere generated a 3 KB eDrawing file at the lowest shaded quality setting, and a 53 KB file at the highest setting. The same test run for a 1″ cube showed no difference in file size (1 KB), since the number of display facets only increases for curved surfaces.
The number of views in the drawing can affect the eDrawing size, but not drastically. Only one 3D representation of the model is saved, regardless of how many drawing views there are. Less views require less line/arc/spline data to be stored, but this data is very compact compared to the 3D image.
With eDrawings Professional, you can choose to include multiple configurations or drawing sheets in the eDrawings you publish. This increases file size but is more efficient than creating multiple eDrawing files for each configuration or drawing sheet.
The option to allow STL creation from an eDrawing file does not appear to increase file size in our experience.
How do You Put a Perspective View on a Drawing?
The icon that changes display mode to “Perspective” within parts and assemblies is not available within the drawing environment, however it is possible to place a perspective view into a drawing. To show a drawing view with perspective (so the part appears tapered toward a vanishing point on the horizon), you need to create a custom view in the model file (part or assembly).
1. Open the model.
2. Go to View – Display – Perspective.
3. Zoom/Pan/Rotate to position the model as you wish.
4. Hit the spacebar to bring up the View Orientation dialog box.
5. Click the icon that looks like a blue telescope with an orange starburst behind it. This allows you to save the current view settings in the file. Type in a name for your custom view.
6. Create or open a drawing of the part/assembly.
7. Choose Insert – Drawing View – Model View, and choose your custom view name from the list of possible views to place on the sheet.
My Drawing Template no Longer Prompts Me for the Paper Size or Titleblock Format to Use. How do I get this Prompt Back?
When you create a Drawing Template (File – Save As – *.drwdot), that template will contain the Sheet Format that existed in the drawing at the time of the Save As. If you would like SolidWorks to prompt you to choose a Sheet Format every time you start a new drawing, you must save a Drawing Template that does not have a Sheet Format in it. Here’s how:
Open a new drawing file using the desired template. [Cancel the Model View command or View Palette if necessary.] Now, in the FeatureManager, click the little “+” next to the icon for “Sheet1″. Now select and delete “Sheet Format1″. Now choose File – Save As – Drawing Templates (*.drwdot). Make sure to save the template file into the folder with the rest of your document templates, overwriting the original if you wish.
3rd Angle vs 1st Angle Projection in Drawings
If the Projected View command creates a Top view of your part below the Front view instead of above it, you are probably experiencing 1st Angle Projection instead of 3rd Angle Projection which is much more common in the USA.
This setting is one of the Sheet Properties. To change it, right-click on the drawing sheet and choose Properties… You will then see a radio button choice where you can switch from 1st Angle Projection to 3rd Angle Projection.
You should now use Save As to save a corrected version of your Drawing Template (see other tech tip above), since the 3rd Angle Projection setting depends on the settings of the Drawing Template for new drawing files.