Technical Tips & Techniques

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» General Tips:

  • Save soon / Save often
    • Autosave activates upon first save
  • Pick plane or face before Insert Sketch
  • Define 3D orientation with 1st profile sketch and sketch plane
  • Keep standard 3 planes in middle of part (midplane)
  • One sketch per feature
  • Dimension sketches and features as in drawing
  • Dimension sketches and features as manufactured
  • Mirror entities in sketch whenever possible
  • Mirror features whenever possible
  • Ctrl click for multiple picks
  • Use feature fillets versus sketch fillets when possible
  • Leave fillets for last if possible
  • Sketch button
    • Starts sketch on last picked face or plane
    • Exits sketch if in sketch
    • Enters and Edits selected sketch
  • Rebuild button
    • Exits sketch and rebuilds parts
  • Use automatic relations whenever possible
  • Use manual relations in place of dimensions when possible
  • Use Link Values when possible
  • Sketch on part faces whenever possible
  • Dimension Colors
    • Blue: Feature dimensions
    • Black: Sketch dimensions
    • Red: Overdefined dimensions
    • Tan: Dangling dimensions
  • Use centerlines if needed
  • Sketch in continuous loop or chain when possible
    • Use inferences versus construction lines
  • Use "thin feature" when possible.

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» Installation:

  • Put macro folder back under SolidWorks directory
  • Point SolidWorks to SW Templates
    • Tools - Options - File Locations - …
  • Point SolidWorks to SW Palette
    • Tools - Options - File Locations - …
  • Execute / Import Copy-Options reg file
  • Put .cus file back under SolidWorks/User directory
  • Set up toolbars

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» Sketch info:

  • Sketch lines
    • Blue lines: Under defined
    • Black lines: Fully defined
    • Red lines: Over defined
    • Tan lines: Dangling
  • Sketch symbols in feature tree
    • Under defined sketch: (-) symbol
    • Fully defined sketch: No symbol
    • Over defined sketch: (+) symbol
  • Inference Lines in sketch
    • Blue (dotted): Informative
    • Tan (dotted): Automatic relations
  • Cursor Image
    • Pink/Orange: Automatic Relation (coincident)

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» Sketch Tips:

  • Hover over curved feature to 'wake up' centerpoint
  • Create automatic relationships (after geometry crEngatechon) by dragging geometry endpoint
  • Moving sketch geometry / entities
    • Move blue entities to visualize underdefined entities
    • Move circle center point to change position
    • Move circle arc to change size
    • Exaggerate move and then return for short distances
  • ALWAYS have fully defined sketches upon design completion

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» Editing:

  • Edit sketch of feature: RMB menu ' "Edit Sketch
    • To change shape of feature
  • Edit feature: RMB menu ' "Edit Definition"
    • To change definition type (e.g. blind, midplane, ect), direction of feature
  • Edit sketch plane: RMB menu ' "Edit Sketch Plane"
    • To move sketch to alternate face or plane

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» Assembly:

  • First part in assembly is automatically fixed
  • Align part and assembly origins automatically by dragging component onto assembly origin
  • Set Selection Filter to Faces for ease of face selection
  • Use Move Tool to visualize degrees of freedom

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» Reorient Standard Views:

  • Sometimes it is beneficial to reorient your standard views on a part so that a typical, three-view drawing will display as required.
  • Orient your 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).
  • Turn on the View Orientation tool by hitting the space bar or clicking on the View toolbar.
  • Select *Front from the list (don't double-click) and click Update Standard Views.

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» Mate References:

  • Applying mate references can speed up the process of adding common parts to assemblies. Mate references establish the connection type for drag & drop smart mates. The mate reference must be saved in the part itself.
  • Open the desired part and select your mate reference.
  • Select Tools, Mate Reference from the menu.
  • Optional: Save the part in a Palette Parts folder for quick access.
  • To use a part with 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).

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» Bogus Parts for Non-Modeled Materials:

You can create parts without any geometry to be used to fill out assemblies and their corresponding BOMs such as grease, paint or wire. Use file properties to fill out extra descriptions, material properties, vendors or any other required BOM information. Simply drag & drop them into any assembly to add them to the BOM. (Hint: Save them in your Feature Palette Parts folder for easy access).

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» Lightweight Parts:

You can improve performance of large assemblies significantly by using lightweight parts. Loading an assembly with lightweight parts is faster than loading the same assembly with fully resolved parts.

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

To enable lightweight loading of parts:

  • Click Tools, Options. On the System Options tab, click Performance.
  • Under Assemblies, select the Automatically load parts lightweight check box.
  • You can set this option with an assembly open; in earlier versions of SolidWorks, you had to close all assemblies first.

To open an assembly with lightweight parts:

  • Click File, Open.
  • The Open dialog box appears.
  • Select the Lightweight check box, browse to the assembly file, and click Open.
  • When this check box is selected, all parts are loaded lightweight when you open an assembly. The only exception is that any parts that are included in the feature scope of an 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.

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» Image Quality:

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

  • With an 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).
  • Select the Image Quality category.
  • Set the Image Quality to Custom and drag the slider bar all the way to Faster.
  • Turn on the check to Apply to all referenced part documents.
  • Save the assembly.

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» Dynamic Drawing View Activation:

In 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 drawing related to a View, the View must be active prior to crEngatechng 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 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:

  • Once a View is added to the Sheet, the Sheet can only be active by right-clicking on it and selecting Lock Sheet Focus.
  • To activate a specific view, right-click on it and select Lock View Focus.
  • 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. (Sometimes this is not what you might want - so use item 2 to ensure appropriate behavior).
  • 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).
  • 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).
  • A selected view (green highlight) is not necessarily active (gray shading on the View border).

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» 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 2001, SolidWorks Explorer. SolidWorks Explorer can be installed freely on any computer (great for document management).

Change revision of a part and its related drawing:

  • In SolidWorks Explorer, click File, Open and browse to the drawing file.
  • Right-click on the drawing in the tree view and select Copy or select Copy from the Edit menu.
  • Turn on the Copy children check box in the copy dialog (this will copy the drawing and the associated parts and/or assemblies).
  • Optional: Click Browse to the right of the Folder box to specify a new folder.
  • Add a suffix or prefix to the file name as per your company standards.
  • Click Apply.
  • Open the new drawing in SolidWorks and make the desired modifications.

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