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SolidWorks tips and tricks
Click here to upload a .pdf on What's New in SolidWorks 2010.
Click here to upload a .pdf on What's New in SolidWorks 2011.
SolidWorks has numerous improvements and features that can aid designers, engineers and students to create and document their ideas quicker and more efficiently. It’s the small things in life that can help you the most and it seems that SolidWorks agrees.
Modify SolidWorks default Templates
A common question is; if the Network Administer loaded SolidWorks with the first default system settings - how can I modify the default Part, Assembly and Drawing document Templates? Below is a procedure to modify the default units and angle type projection:
For a Part Document:
Click File, New from the Main menu
Double-click Part document
Click Tools, Options, Document Properties
Click Units
Select Unit type, (IPS)
Click OK
Click File, Save As from the Main menu
Select Part Templates from the Save as type drop-down menu as illustrated
Click Part.prtdot as the file name as illustrated.
Click Save
Close all documents. This is a very important step. Next time you create a new Part document - it will use your modifications.
For an Assembly Document:
Follow the above procedure and click Assembly as the file name.
Close all documents. This is a very important step. Next time you create a new Assembly document - it will use your modifications.
For a Drawing Document:
Click File, New from the Main menu
Double-click Drawing document
Select Sheet Format - (A size)
Click Cancel from the Model View PropertyManager
Right-click Properties in the drawing sheet
Click Third angle for type of projection as illustrated
Click OK from the Sheet Properties dialog box
Click Tools, Options, Document Properties
Click Units
Select Unit type, (IPS)
Click OK
Click File, Save As from the Main menu
Select Drawing Templates from the Save as type drop-down menu as illustrated
Click Drawing.drwdot.
Click Save
Close all documents. This is a very important step. Next time you create a new Drawing document - it will use your modifications.
Context Toolbars - Customize
You may want to customize the shortcut toolbar. The context toolbars are document dependent; sketch, part, assembly, and drawing.
Step1: Activate the shortcut toolbar. Note: Press the "S" key with nothing selected in the Graphics window.
Step2: Right-click the Context toolbar.
Step3: Click Customize. The Customize dialog box is displayed.
Step4: To customize the sketch context toolbar, click the Commands tab, click Sketch. The available Sketch toolbar are displayed. Note: You can select any Catagory to add to the shortcut toolbar.
Step5: Click and drag the required Sketch tool icon to the context toolbar as illustrated. Note: You can click and drag as many tool icons to the shortcut toolbar. To remove an icon, click and drag it back to the Customize dialog box.
Step6: Click OK from the Customize dialog box to finish.
Mouse Gestures
The mouse gestures tool provides the ability to access commonly used commands. Users can choose to have four or eight shortcuts on the mouse gesture guide.
The mouse gesture guide is displayed when you Right-click in the Graphics window and drag the mouse pointer icon to the desired command.
You can customize the gestures independently for any commands in the sketch, part, assembly, and drawing document.
If desired; the mouse gestures guide can be deactivated by going to clicking Tools, Customize, and uncheck the option on the Mouse Gestures tab.
Adding a Watermark to your Drawing
A CONFIDENTIAL Watermark may be required on a drawing. At this time, SolidWorks does not offer a Watermark tool. Below are two ways to create a workaround.
First Way: Apply an MS Word Watermark
Step1: Open a drawing.
Step2: In the active Sheet, right-click Edit Sheet Format.
Step3: Click Insert, Object from the Menu bar menu. The Insert Object dialog box is displayed. Note: You can also add company logos this way.
Step4: Select MS Word Picture from the Drop-down menu.
Step5: Click OK. A MS Word document is displayed. Picture in Drawing# - Sheet#.
Step6: Click Format, Background, Printed Water Mark from the Main menu in the MS Word document.
Step7: Insert a Text Water Mark. Check the Text watermark box.
Step8: Select the Text from the drop-down box or enter your own text as illustrated. Note: To insert a picture, click the Picture watermark box, and select your picture.
Step9: Set the required Font size and type.
Step10: Click OK from the Printer Watermark dialog box.
Step11: Click Close picture as illustrated. The Watermark is displayed in the active sheet.
Step12: Size the Watermark to your sheet.
Step13: Right-click Edit Sheet to return to the active drawing mode. Note: Do not click inside the Watermark!
Second Way: Create a Block.
Step1: Open a drawing.
Step2: In the active Sheet, Right-click Edit Sheet Format.
Step3: Click the Note tool from the Annotate tab located in the CommandManager. The Note PropertyManager is displayed.
Step4: Click the location on the Sheet for the Watermark.
Step5: Enter the Watermark text, font, color, options needed.
Step6: Click OK from the Note PropertyManager.
Step7: Right-click the note in the drawing Sheet. Note: You are in the Edit Sheet Format mode.
Step8: Click Make Block. The Make Block PropertyManager is displayed.
Step9: Click OK from the Make Block PropertyManager.
Step10: Right-click Edit Sheet to return to the active drawing mode. The Watermark is created.
*Assembly Tips
Use the default reference planes of the components to mate to
The default reference planes are always there and they do not change even if the geometry changes.Rename the default reference planes Rename the planes to make them more relevant.
Mate to the first component added in the assembly
If you mate to the first component or base component of the assembly and then decide to modify the orientation later, all the components will move with it.Mate hardware stacks together
Always think of the future - Design Intent. Desgin for change. If you have to modify the location or loose a reference to a hole or slot - this will save you modeling time.Mate components together that move together
The angle and fastener moves with the bar, so go ahead and mate them to it.Create sub-assemblies that you can drop and dissolve
Instead of mating in the same thing over and over again, create an assembly that has everything in it already, drop it in your main assembly, right click and dissolve it.Create a simple fully constrained configuration to help models load faster
This configuration can have things like hardware, internal parts and assembly cuts suppressed.Create folders to organize parts, fastners, components and sub-assemblies in the FeatureManager
This just helps keep things organized and easier to find. Select a group of parts or assemblies, right click one of them and select Add to folder. Then give it a good name.Create component descriptions in the FeatureManager
Create smart parts - which will be smart components in an assembly. Start with the part description, and add Custom properties. Right click on the Assembly name in the FeatureManager, click Tree Display, Show Component Description. This is extremely helpful if your documents are named with numbers and can give you a look at how your BOM will be appeared either in the Assembly or Drawing.Apply component patterns
This starts at the part level too. Use linear, circular, sketch driven or hole wizard patterns in your parts. This makes your job easier in the assembly by allowing you to use Component Patterns.Create an empty part for ambiguous parts
The part should have a small extruded feature in it so you can give it a mass. You can hide the body in the Solid Bodies folder in the FeatureManager. This can help if you need exact measurements of ambiguous parts like adhesive, insulation or water.Use Isolate when editing parts
If you right click on a part in an assembly, select Isolate. This hides all the other parts. Then, you can edit without all the other stuff getting in the way.*Information obtained from SolidSmack.
New Office Products tab in SolidWorks 2011
Provides the ability to directly insert key Add-ins.
Some of the best SolidWorks tips to teach someone:
New documents get their document settings (such as units, image quality, etc.) from the document properties of the template used to create the model or drawing.
Model about the origin, this is great for a new user because it provides a point of reference.
If possible, keep your base sketch simple.
Add relations, then dimensions. This will keep the user from having too many unnecessary dimensions. This helps to show the design intent of the model. Dimension what geometry you intent to modify or adjust.
Link Dimensions. Select two dimensions, right-click and select Link Values to control both dimensions. Think of a cube. Link all dimensions controlling it, you modify one and the cube is updated.
Use Symmetry. When possible and if it makes sense, model objects symmetrically about the origin. Even if the part is not symmetrical, the way it attaches or is manufactured will have symmetry.
Build design intent into a feature by addressing End Conditions (Blind, Through All, Up to Next, Up to Vertex, Up to Surface, Offset from Surface, Up to Body and Mid Plane) symmetry, feature selection, and the order of feature creation.
The basic End Conditions are:
- Blind - Extends the feature from the selected sketch plane for a specified distance - default End Condition.
- Through All - Extends the feature from the selected sketch plane through all existing geometry.
- Up to Next - Extends the feature from the selected sketch plane to the next surface that intercepts the entire profile. The intercepting surface must be on the same part.
- Up To Vertex - Extends the feature from the selected sketch plane to a plane that is parallel to the sketch plane and passing through the specified vertex.
- Up To Surface - Extends the feature from the selected sketch plane to the selected surface.
- Offset from Surface - Extends the feature from the selected sketch plane to a specified distance from the selected surface.
- Up To Body - Extends the feature up to the selected body. Use this option with assemblies, mold parts, or multibody parts.
- Mid Plane - Extends the feature from the selected sketch plane equally in both directions.
When you create a new part or assembly, the three default Planes (Front, Right and Top) are align with specific views. The Plane you select for the Base sketch determines the orientation of the part.
The three default Reference planes represent infinite 2D planes in 3D space. Planes have no thickness or mass.
Sketches are generally in one of the following states:
- Under defined - Prefix (-) The sketch is displayed in red.
- Fully defined - No prefix The sketch is displayed in black.
- Over defined - Prefix (+) The sketch is displayed in blue.
Fully define your sketch when possible.
Add relations, then dimensions. This keeps the user from having too many unnecessary dimensions. This also helps to show the design intent of the model. Dimension what geometry you intent to modify or adjust.
Rename a feature or sketch for clarity. Slowly click the feature or sketch name twice and enter the new name when the old one is highlighted.
By default, the Dimension tool utilizes the center point of an arc or circle. Select the circle profile during dimensioning. Utilize the Leaders tab in the Dimension PropertyManager to modify the arc condition to Minimum or Maximum.
Utilize the Hole Wizard feature when creating non Through All complex geometry holes.
Apply construction reference geometry to assist in creating the sketch entities and geometry that are incorporated into the part. Construction reference geometry is ignored when the sketch is used to create a feature. Construction reference geometry uses the same line style as center lines.
Utilize the Save As command and work on the copied version of the document before making any changes to the original. Keep the original document intact.
Use Symmetry. When possible and if it makes sense, model objects symmetrically about the origin. Even if the part is not symmetrical, the way it attaches or is manufactured will have symmetry.
An object is symmetrical when it has the same exact shape on opposite sides of a dividing line (or plane) or about a center or axis. The simplest type of Symmetry is a “Mirror” as we discussed above in this chapter.
Symmetry can be important when creating a 2D sketch, a 3D feature or an assembly. Symmetry is important because:
- Mirrored shapes have symmetry where points on opposite sides of the dividing line (or mirror line) are the same distance away from the mirror line.
- For a 2D mirrored shape, the axis of symmetry is the mirror line.
- For a 3D mirrored shape, the symmetry is about a plane.
- Molded symmetrical parts are often made using a mold with two halves, one on each side of the axis of symmetry.
- The axis or line where two mold parts join is called a parting line.
Customize the CommandManager
The CommandManager was introduced in 2006. The CommandManager is a context-sensitive toolbar that dynamically updates based on the toolbar you want to access. By default, it has toolbars embedded in it based on the document type; part, drawing, assembly.
The default CommandManager for a part document using SolidWorks Premium is:
Display or Hide a tab on the CommandManager:
Step1: Right-click any of the CommandManager tabs. A dialog box is displayed as illustrated.
The dialog box displays the availalble toolbars for the active document.
Step2: Uncheck the tools to be hidden, and check the tools to be displayed. Note: The Customize CommandManager tool provides access to the Customize dialog box.
Reorder the tabs in the CommandManager:
The dialog box displays the availalble toolbars for the active document
Step1: Right-click any of the CommandManager tabs. A dialog box is displayed as illustrated.
Step2: Check the Customize CommanManager tool. The Customize dialog box is displayed.
Step3: Click and drop any tab in the desired location.
Step4: Click OK from the Customize dialog box.
Add a new tab to the ComandManger:
Step1: Right-click any of the CommandManager tabs. A dialog box is displayed
Step2: Check the Customize CommanManager tool. The Customize dialog box is displayed.
A new tab icon is displayed in the CommandManager tab row.
Step3: Enter the name of the new tab or right-click to rename the tab.
Step4: Click OK from the Customize dialog box. The new tab is displayed.
Reset the CommandManger to the default settings:
Step1: Right-click any of the CommandManager tabs. A dialog box is displayed.
Step2: Check the Customize CommanManager tool. The Customize dialog box is displayed.
Step3: Click the Options tab.
Step4: Click the Reset to Default buttons.
Step5: Click OK from the Customize dialog box.
D&M Education LLC
Hopkinton, MA 01748
United States
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