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Top 10 underused features in SolidWorks

This technical tip highlights key SolidWorks® capatiblities that are sometimes overlooked by even the most experienced SolidWorks users.

Sketching

Sketch relations filter

You can use the relations filter in the display/delete relations property manager to view specific subsets of relations instead of getting a list of every relation in the sketch. You can filter the relations list to show only the Dangling, Overdefining/Not Solved, External, Defined in Context, Locked, Broken, or Selected Entities.

For instance, if you are trying to remove in-context relations from a sketch, it is much faster to select the ‘defined in-context' filter instead of searching through the complete list to manually find all relations with the ‘->' symbol.

When changes in a model cause a child sketch to show rebuild errors, one or more of the sketch's external relations must have caused the errors.   You can quickly find and repair the cause of the problem by filtering for external relations in the display/delete relations dialog.

Sketch-modify

When a sketch plane is redefined or when a sketch is copied and pasted onto a new face/plane, the sketch may get rotated or mirrored. To quickly reorient sketches that do not have external relations, Click Tools/Sketch Tools/Modify. Right-clicking the black ends of the cursor will flip a sketch along that axis. Right-click-drag anywhere on the screen will rotate the sketch, or you can enter a rotation value in the dialog box.

Projected curve

It is easier to create, control, and manipulate 3D curves by using a projected curve instead of a 3D sketch. Any curve that can be fully described in just two orthogonal views can be created by projecting one 2D sketch onto a second 2D sketch. Just select the ‘sketch on sketch' option in the projected curve dialog.

Intersection curve

You can instantly create sketch geometry where the cross-section of a face, body, or entire model intersects a sketch plane with intersection curve. You can also use intersection curve to create 3D sketch curves from the intersection of faces, bodies, and models.

Sketches for calculations

You shouldn't limit using the SolidWorks sketcher to creating feature geometry — you can also use the SolidWorks sketcher to solve geometric and trigonometry problems. For instance, you can use a sketch to calculate the horizontal and vertical components of an angular force, or you could create a sketch to work out the maximum possible rib height given a draft angle, minimum thickness at the top, and maximum thickness at the root.  

Dimension placement

The smart dimension tool automatically changes the included angle of an angular dimension or the type of linear dimension (horizontal, vertical, or projected) based on where you left-click to place the dimension. To lock the included angle/linear dimension type before you place it, move the cursor to obtain the correct dimension appearance then right-click. You can then place the dimension at the desired location without having that placement change how the dimension reads. Right-clicking again before placing the dimension will revert it to its original behavior.

Arc length

You can add a dimension to drive an arc's length by clicking the two ends of the arc then clicking the body of the arc before placing the dimension

Angle between points

You can dimension the angle between two points in relation to a third.   Select the point for the vertex of the angle, and then select the other two points before placing the dimension.

Part Modeling

Part validation: Verification on rebuild controls the level of error checking performed on a model. It is off by default to promote faster rebuild of the model; however, this means that some errors in the model will not be caught immediately. When working on more complicated geometry, turn on verification on rebuild to avoid unidentified errors that can eventually jeopardize additional model features.

Draft and design intent: Neutral plane draft calculates the intersection of the selected face and the neutral plane and angles the face relative to that intersection (central image in the image below). Note how the upper red face in that image no longer corresponds with its original dimension.  

To add draft to a face but keep it locked to its original design intent use a parting line draft. Parting line draft angles a face relative to any adjacent edge (shown in red in the right side image of figure X), not just the parting line of the model.

Extrude to direction vector

To correctly build features built on drafted faces, you can specify a direction vector for the extrusion

Change colors

Assign colors to sketches, projected curves and composite curves to make them easier to find and differentiate on screen

Ruled Surface

This feature can take an edge or collection of edges and generate a single or collection of ruled surfaces – think of radiate surface with many more options. The ruled surfaces may be tangent to the adjacent faces, normal to them, tapered towards or perpendicular to a specified vector, along an edge (sweep) or defined by the co-ordinate system.

Assemblies:

Component descriptions

If you have trouble finding specific components in an assembly when every component is named with a part number, you can opt to have the tree show the components by their description. At the top of the FeatureManager™ design tree, right-click the assembly name and select Tree Display, Show Component's Description

Drawings:

Faster drawings: Using shaded views increases drawing performance over wireframe and hidden line views. If the final drawing needs to be wireframe or hidden line, you should complete all the detailing in shaded mode then convert the views to the desired mode only at the end of the job.

Inserting model items

Expanding the drawing view in the drawing manager allows you to access the feature tree of the models in that view. You can highlight individual features to cleanly insert model items into the correct view one feature at a time.  

Font changes

Activate the Font toolbar to quickly change the size and style of annotations.

Black and white printing

By default, driven dimensions show as gray in drawings and will print as gray. To make the driven dimensions and all other gray items print black, select ‘black and white' as your drawing color in page setup.

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