engatech

Quick Links: SolidWorks General Tips SolidWorks Installation SolidWorks Sketch Info SolidWorks Sketch Tips SolidWorks Editing SolidWorks Assembly SolidWorks Reorient Standard Views	SolidWorks Mate References SolidWorks Virtual Parts for Non-Modeled Materials SolidWorks Lightweight Parts SolidWorks Image Quality SolidWorks Dynamic Drawing View Activation SolidWorks Explorer SolidWorks Tips & Tricks Newsletters

» SolidWorks General Tips:

1. 1. Save soon / Save often
           a. Autosave activates upon first save
   2. Pick plane or face before Insert Sketch
   3. Define 3D orientation with 1st profile sketch and sketch plane
   4. Keep standard 3 planes in middle of part (midplane)
   5. One sketch per feature
   6. Dimension sketches and features as in SolidWorks drawing
   7. Dimension sketches and features as manufactured
   8. Mirror entities in sketch whenever possible
   9. Mirror features whenever possible
   10. Ctrl click for multiple picks
   11. Use feature fillets versus sketch fillets when possible
   12. Leave fillets for last if possible
   13. Sketch button
           a. Starts sketch on last picked face or plane
           b. Exits sketch if in sketch
           c. Enters and Edits selected sketch
   14. Rebuild button
   15. Exits sketch and rebuilds parts
   16. Use automatic relations whenever possible
   17. Use manual relations in place of dimensions when possible
   18. Use Link Values when possible
   19. Sketch on part faces whenever possible

   20. Dimension Colors (See Below Image)         a. Blue: Feature dimensions         b. Black: Sketch dimensions         c. Yellow: Overdefined dimensions         d. Tan: Dangling dimensions         e. Gray: Reference Dimensions

   21. Use centerlines if needed
   22. Sketch in continuous loop or chain when possible
   23. Use inferences versus construction lines
   24. Use "thin feature" when possible.

Back to Tip List

» SolidWorks Installation:

1. Put macro folder back under SolidWorks directory
2. Point SolidWorks to SW Templates
        a. Tools - Options - File Locations - …
3. Point SolidWorks to SW Palette
        a. Tools - Options - File Locations - …

• 4. Using Copy Settings Wizard, Execute / Import Copy-Options reg file

Back to Tip List

» SolidWorks Sketch Info:

• 1. SolidWorks Sketch lines (See Below Image)       a. Blue lines: Under defined       b. Black lines: Fully defined       c. Yellow lines: Over defined       d. Tan lines: Dangling

  2. SolidWorks Sketch symbols in feature tree (See Below Image)       a. Under defined sketch: (-) symbol       b. Fully defined sketch: No symbol       c. Over defined sketch: (+) symbol

  3. SolidWorks Inference Lines in sketch (See Below Image)       a. Blue (dotted): Informative       b. Yellow (dotted): Automatic relations

  4. SolidWorks Cursor Image (See Above Image)       a. Yellow: Automatic Relation (coincident)       b. White: Informative

Back to Tip List

» SolidWorks Sketch Tips:

1. Hover over curved feature to 'wake up' centerpoint

2. Create automatic relationships (after geometry creation) by dragging geometry endpoint

3. Moving SolidWorks sketch geometry / entities

       a. Move blue entities to visualize underdefined entities

       b. Move circle center point to change position

       c. Move circle arc to change size

       d. Exaggerate move and then return for short distances

• 4. ALWAYS have fully defined SolidWorks sketches upon design completion.

Back to Tip List

» SolidWorks Editing:

1. Edit sketch of feature: left click or RMB select the image sketch image “Edit Sketch”        a. To change shape of SolidWorks feature  (See Below Image)

2. Edit feature: left click or RMB select image of a finger over an extrude command “Edit Feature”        a. To change definition type (e.g. blind, midplane, ect), direction of feature  (See Below Image)

3. Edit sketch plane: left click or RMB select image of a finger over the plane symbol “Edit Sketch Plane”        a. To move SolidWorks sketch to alternate face or plane

Back to Tip List

» SolidWorks Assembly:

1. First part in SolidWorks assembly is automatically fixed

2. Align part and SolidWorks assembly origins automatically by dragging component onto SolidWorks
    assembly origin

3. Set Selection Filter to Faces for ease of face selection

4. Use Select Other to select through faces versus rotating

• 5. Use Move Tool to visualize degrees of freedom

Back to Tip List

» SolidWorks Reorient Standard Views:

1. Sometimes it is beneficial to reorient your SolidWorks standard views on a part so that a typical, three-
    view drawing will display as required.

2. Orient your SolidWorks part to what should be the front view. (Hint: You can use Normal To views by
    selecting a face to view normal to and then control-select a face that represents the vertical direction
    of the new view. This will cause the Normal To view to turn appropriately).

3 Turn on the View Orientation tool by hitting the space bar or clicking on the View toolbar.

4. Select *Front from the list (don't double-click) and click Update Standard Views.

Back to Tip List

» SolidWorks Mate References:

• 1. Applying SolidWorks mate references can speed up the process of adding common parts to assemblies.
      SolidWorks Mate references establish the connection type for drag & drop smart mates. The
      SolidWorks mate reference must be saved in the part itself.

  2. Open the desired part and select your SolidWorks mate reference.

  3. Select Tools, Mate Reference from the menu.

  4. Optional: Save the part in a Palette Parts folder for quick access.

  5. To use a part with SolidWorks mate references, drag & drop the part from either a Windows Explorer
      folder, the Feature Palette or from the part icon of the open part. When you drag it, watch for the
      preview image to verify position and alignment condition. (Hint: To flip the alignment condition, use
      the Tab key before releasing your mouse button).

Back to Tip List

» SolidWorks Virtual Parts for Non-Modeled Materials:

You can create SolidWorks virtual parts without any geometry to be used to fill out SolidWorks assemblies and their corresponding Bills of Material such as grease, paint or wire. Use file properties to fill out extra descriptions, material properties, vendors or any other required BOM information. Or save them in design library and simply drag & drop them into any SolidWorks assembly to add them to the BOM. Using virtual parts means you do not have another file to manage.

Back to Tip List

» SolidWorks Lightweight Parts:

• You can improve performance of large SolidWorks assemblies significantly by using lightweight parts. Loading a SolidWorks assembly with lightweight parts is faster than loading the same SolidWorks assembly with fully resolved parts. SolidWorks lightweight parts are efficient because the full model data for the parts is loaded only as it is needed. Only parts that you select, and parts that are affected by changes that you make in the current editing session, become fully resolved.

  Assemblies with SolidWorks lightweight parts rebuild faster because less data is evaluated. SolidWorks Mates on a lightweight part are solved, and you can edit existing SolidWorks mates.

  To enable SolidWorks lightweight loading of parts:

  1. Click Tools, Options. On the System Options tab, click Performance.

  2. Under SolidWorks Assemblies, select the Automatically load parts lightweight check box.

  3. You can set this option with an assembly open; in earlier versions of SolidWorks, you had to close all
      assemblies first.

  To open a SolidWorks assembly with lightweight parts:

  1. Click File, Open.

  2. The Open dialog box appears.

  3. Select the Lightweight check box, browse to the SolidWorks assembly file, and click Open.

  4. When this check box is selected, all parts are loaded lightweight when you open an SolidWorks assembly.
      The only exception is that any parts that are included in the feature scope of an SolidWorks assembly
      feature are always loaded fully resolved (see Assembly Features). Sub-assemblies themselves are not
      loaded lightweight, but the individual parts that they contain are lightweight.

  As of 2009, all assembly drawings load lightweight. This allows drawings to load faster and doesn’t require as much memory to load a drawing.

Back to Tip List

» SolidWorks Image Quality:

You can dramatically reduce file size, decrease open and save times and increase rotational performance of larger SolidWorks assemblies by modifying the image quality.

1. With an SolidWorks assembly open, select Tools, Options and then select the Document Properties
    tab (Hint: To quickly access Document Properties, right-click in a blank space in the Feature Manager
    design tree).

2. Select the Image Quality category.

3. Set the Image Quality to Custom and drag the slider bar all the way to Faster.

4. Turn on the check to Apply to all referenced part documents.

5. Save the SolidWorks assembly.

Back to Tip List

» SolidWorks Dynamic Drawing View Activation:

In SolidWorks drawings there are several "containers" for added text and sketch geometry. These include Views, Sheets and Sheet Formats. However, only one can be actively used at a time. For example, if you want to place some text on your SolidWorks drawing related to a View, the View must be active prior to creating the text. If you want the text on the drawing Sheet, the Sheet must be active first. If you want the text on the Sheet Format (or titleblock), the Sheet Format must first be active

Most users are familiar with the difference between Edit Sheet and Edit Sheet Format modes in SolidWorks drawings. When you edit the Sheet Format, it ensures that anything added will be on the Sheet Format and not on the Sheet. However, determining whether added objects are related to the Sheet or a View is a little more complicated. Here are a few items to remember:

1. Once a View is added to the Sheet, the Sheet can only be active by right-clicking on it and selecting
    Lock Sheet Focus.

2. To activate a specific view, right-click on it and select Lock View Focus.

3. To unlock focus to a View or the Sheet, double-click on any view. By default, Views activate as you
    move your mouse around the screen so that the View closest to your mouse is always active.

4. Automatic View Activation is an optional setting. It is located in Tools, Options - System Options,
    Drawings. If it is turned off, the behavior for activation of views is through a double-click (the same
    as SolidWorks 98 and previous versions).

5. If you can't select sketch geometry on a drawing, it is probably connected to a different View than
    the one you have currently active. Lock View Focus for each View until the sketch geometry becomes
    available to select (or possibly lock the Sheet Focus).

6. A selected view (green highlight) is not necessarily active.

Back to Tip List

» SolidWorks Explorer:

SolidWorks Explorer is an excellent tool for copying, renaming and managing SolidWorks files while maintaining file references. You can access SolidWorks Explorer either from the Tools menu in SolidWorks or through Start, Programs, SolidWorks 20**, SolidWorks Explorer. SolidWorks Explorer can be installed freely on any computer (great for document management).Change revision of a part and its related drawing:

1. In SolidWorks Explorer, click File, Open and browse to the drawing file.

2. Right-click on the SolidWorks drawing in the tree view and select Copy or select Copy from the Edit
    menu.

3. Turn on the Copy children check box in the copy dialog (this will copy the drawing and the associated
    parts and/or assemblies).

4. Optional: Click Browse to the right of the Folder box to specify a new folder.

5. Add a suffix or prefix to the file name as per your company standards.

6. Click Apply.

7. Open the new drawing in SolidWorks and make the desired modifications.

Back to Tip List

» SolidWorks Tips & Tricks Newsletters:

• Subscribe to the SOLID Digital Digest Newsletter - SOLID Solutions magazine's free weekly newsletter for SolidWorks users
  http://www.solidmag.com/


• SolidWorks Tips and Things email newsletter
  http://www.solidworktips.com/tip_sign_up.htm


• SolidWorks Community Newsletter:
  http://www.solidworks.com/swexpress/index.html


• E-Mail Sign up:
  http://www.solidworks.com/pages/company/Opt-informs/Public_Opt-In.html

Back to Tip List

Privacy Policy