{"id":14734,"date":"2023-03-27T17:14:36","date_gmt":"2023-03-27T21:14:36","guid":{"rendered":"https:\/\/blogs.solidworks.com\/teacher\/?p=14734"},"modified":"2023-04-12T08:45:14","modified_gmt":"2023-04-12T12:45:14","slug":"solidworks-xdesign-lesson-10-sketching-constraints-dimensions","status":"publish","type":"post","link":"https:\/\/blogs.solidworks.com\/teacher\/2023\/03\/solidworks-xdesign-lesson-10-sketching-constraints-dimensions.html","title":{"rendered":"SOLIDWORKS xDesign Lesson #10: Sketching, Constraints, Dimensions"},"content":{"rendered":"

\u00a0\u00a0 \u00a0 \u00a0 After teaching 1000’s of students and writing about SOLIDWORKS for over 25 years, David Planchard, emeritus WPI, is exploring xDesign.\u00a0 Through the SOLIDWORKS xDesign Lesson series, David helps educators understand the differences and similarities between xDesign and SOLIDWORKS through simple examples. He also introduces new apps in the engineering design process. \u00a0 \u00a0\u00a0\u00a0\u00a0\u00a0\u00a0\u00a0 \u00a0<\/em><\/p>\n

One of the most important concepts in CAD modeling is building in the correct design intent.<\/p>\n

Design Intent<\/h2>\n

All designs are created for a purpose. Design intent is the intellectual arrangement of sketches, constraints, dimensions, and features of a design. Design intent manages the relationship between sketches in a feature, features in a part, and parts in an assembly.<\/p>\n

A definition of design intent is the process in which the model is developed to accept future modifications. Models behave differently when design changes occur.<\/p>\n

Build design intent in a sketch as the profile is created. A profile is determined from Sketch entities. Example: Rectangle, Circle, Arc, Point, Slot, etc. Note: <\/strong>xDesign uses the name Sketch entities. SOLIDWORKS uses the name Sketch tools.<\/p>\n

Apply symmetry into a profile through a sketch centerline, mirror entity and position about the reference planes and Origin. Always know the location of the Origin in the sketch.<\/p>\n

\"\"<\/p>\n

You should have a design strategy with your sketch profiles as you create the 3D features for the component.<\/p>\n

Login to the 3D<\/strong>EXPERIENCE platform.<\/p>\n

Start xDesign.<\/p>\n

Click the center of the Compass<\/strong> as illustrated for Roles, Apps & Solutions portfolio.<\/p>\n

\"\"<\/p>\n

Click 3D Designer (3D Creator)<\/strong> under the My Roles (xDesign).<\/p>\n

Click xDesign\u00a0<\/strong>to launch the App. The xDesign App creates components in a single modeling environment. The term component is used because both parts and assemblies are treated the same. This is not true in SOLIDWORKS.<\/p>\n

\"\"<\/p>\n

The default Name* of the component is Physical Product 1.<\/p>\n

The default Location defines the Collaborative space (cloud storage) where your components are saved. This makes it easy to communicate and share designs with your students and team members, regardless of physical location.<\/p>\n

The default Location maybe named: Common Space. Collaborative space location will differ depending on setup.<\/p>\n

The 3DSpace App is used to create Collaborative space locations. The Quick Start xDesign Collaborative space and the 3DEXPERIENCE mouse control is used in the lesson.<\/p>\n

Create a new component<\/h2>\n

Click New Component<\/strong>.<\/p>\n

Rename<\/strong> component to Revolved Pin.<\/p>\n

\"\"<\/p>\n

Click OK<\/strong>.<\/p>\n

The xDesign App is displayed.<\/p>\n

Trimetric Planes xy, yz, zx are located at the center of the Work Area.<\/p>\n

The default axes are: +x, +y, +z<\/p>\n

Create Sketch.1. Sketch.1 is normal to the yz plane (Front). Quick Start xDesign is the Collaborative space. When you create a new component, the three default planes (xy), (yz), (zy) are aligned with specific views. The plane you select for your first sketch determines the orientation of the part. Selecting the correct plane to start your model is very important.<\/p>\n

Click the yz\u00a0<\/strong>plane<\/strong> in the Design Manager.<\/p>\n

Click Create<\/strong> Sketch<\/strong> from the Context toolbar.<\/p>\n

\"\"<\/p>\n

Create a horizontal line through the Origin along the y axis.<\/p>\n

Click Line<\/strong> from the Sketch tab in the Action bar.<\/p>\n

Click a horizontal<\/strong> position to the left<\/strong> of the Origin as illustrated.<\/p>\n

Click a horizontal position to the right<\/strong> through the Origin as illustrated.<\/p>\n

Deactivate the Line entity.<\/p>\n

Press the Esc <\/strong>key. Note<\/strong>: Can can also double-click to deactivate the Line. The sketching process is straight forward as it is in SOLIDWORKS.<\/p>\n

Click the horizont<\/strong>al line<\/strong> as illustrated. The Coincident and Horizontal callout icons are displayed. This is similar in SOLIDWORKS.<\/p>\n

Change the horizontal line to an Infinite line. Use the Infinite line as the axis of revolution for the Revolve Feature. Note<\/strong>: You can also use a Construction line as an axis of revolution. The Construction line must be dimensioned relative to other geometry to be fully defined. This is not the case in SOLIDWORKS.<\/p>\n

\"\"<\/p>\n

Click Infinite line<\/strong> in the Context toolbar.<\/p>\n

\"\"<\/strong><\/p>\n

Create the Sketch profile<\/h2>\n

Click Line<\/strong> from the Action bar.<\/p>\n

Click the Origin<\/strong>. Sketch the first vertical line above the Origin as illustrated.<\/p>\n

Click a point <\/strong>approximately 90mm. A V (Vertical constraint) is displayed during the sketch process.<\/p>\n

\"\"<\/strong><\/p>\n

Sketch a horizontal line<\/strong> from the endpoint of the first vertical line.<\/p>\n

Click a point<\/strong> approximately 80mm. A H (Horizontal constraint) is displayed during the sketch process.<\/p>\n

\"\"
\n<\/strong><\/p>\n

Sketch the second vertical <\/strong>line.<\/p>\n

Click a point <\/strong>approximately 60mm.<\/p>\n

Sketch the second horizontal<\/strong> line.<\/p>\n

Click a point<\/strong> approximately 110mm.<\/p>\n

\"\"<\/p>\n

Complete the sketch profile<\/strong> as illustrated. Note<\/strong>: Create a closed sketch. The end point is the Origin. At this time, do not worry about dimensions for the other lines.<\/p>\n

\"\"<\/p>\n

Deactivate Line.<\/p>\n

Press the Esc<\/strong> key.<\/p>\n

A good practice is to first add sketch constraints and then dimensions to a sketch.<\/p>\n

Add Constraints<\/h2>\n

Add the first Equal constraint to the left and right vertical lines.<\/p>\n

Click the left vertical line<\/strong>. Do not click the midpoint.<\/p>\n

Hold the Ctrl key<\/strong> down.<\/p>\n

Click the right vertical<\/strong> line<\/strong>. Do not click the midpoint.<\/p>\n

Release the Ctrl key<\/strong>.<\/p>\n

\"\"<\/p>\n

Click Equal<\/strong> from the Constraints toolbar.<\/p>\n

Add the second Equal constraint to the top left vertical line and the top right vertical line.<\/p>\n

Click the top left vertical<\/strong> line. Do not click the midpoint.<\/p>\n

Hold the Ctrl key<\/strong> down.<\/p>\n

Click the top right vertical line<\/strong>. Do not click the midpoint.<\/p>\n

Release the Ctrl key<\/strong>.<\/p>\n

Click Equal<\/strong> from the Constraints toolbar.
\n \"\"<\/strong><\/p>\n

Add the third Equal constraint to the left and right horizontal lines.<\/p>\n

Click the left horizontal line<\/strong>. Do not click the midpoint.<\/p>\n

Hold the Ctrl key<\/strong> down.<\/p>\n

Click the right horizontal line<\/strong>. Do not click the midpoint.<\/p>\n

Release the Ctrl key<\/strong>.<\/p>\n

Click Equal<\/strong> from the Constraints toolbar.<\/p>\n

\"\"<\/p>\n

Deselect the constraints.<\/p>\n

Press the Esc<\/strong> key.<\/p>\n

\"\"<\/p>\n

Note:<\/strong> To delete an existing constraint, click on the entity. Click the contraint. Click Delete.<\/p>\n

\"\"<\/p>\n

At this time, Sketch.1 is underdefined. The under define sketch symbol (-) is the same as SOLIDWORKS.<\/p>\n

\"\"<\/p>\n

Dimension the sketch<\/h2>\n

There are many different ways to insert dimensions.<\/p>\n

Click Sketch Dimension<\/strong> from the Action bar.<\/p>\n

\"\"<\/p>\n

Click the right vertical line<\/strong> (not the midpoint).<\/p>\n

Click a position<\/strong> to the right.<\/p>\n

Enter 10<\/strong>.<\/p>\n

\"\"<\/p>\n

Click the second vertical line <\/strong>(not the midpoint).<\/p>\n

Click a position<\/strong> to the left.<\/p>\n

Enter 10<\/strong>.<\/p>\n

\"\"<\/strong><\/p>\n

Click the top horizontal line <\/strong>(not the midpoint).<\/p>\n

Click a position<\/strong> above the line.<\/p>\n

Enter 20<\/strong>.<\/p>\n

Click the bottom horizontal<\/strong> line <\/strong>(not the midpoint).<\/p>\n

Click a position <\/strong>below the line.<\/p>\n

Enter 40<\/strong>.<\/p>\n

Deactivate Sketch Dimension.<\/p>\n

Press the Esc<\/strong> key.<\/p>\n

\"\"<\/p>\n

Sketch.1 is displayed in black and is fully defined.<\/p>\n

Press the f<\/strong> key to fit the sketch to the Work Area.<\/p>\n

Note:<\/strong> To delete a dimension, click the leader line of the dimension. Click Delete from the General Context toolbar.<\/p>\n

\"\"<\/p>\n

Save the component.<\/p>\n

Click Save <\/strong>from the Action bar.<\/p>\n

Create a Revolve feature<\/h2>\n

A Revolve is a sketch base feature. A Revolve feature adds material. The Revolve feature requires an infinite line or centerline and a sketch profile on a Sketch plane. A Revolve feature requires an angle of revolution. The sketch is revolved around the infinite line or centerline.<\/p>\n

Click Revolve<\/strong> from the Action bar.<\/p>\n

\"\"<\/p>\n

The Revolve dialog box is displayed.<\/p>\n

Solid is selected by default.<\/p>\n

Click the Infinite line<\/strong> in the Work Area. Line.1 is displayed in the Select revolve axis box.<\/p>\n

Click Sketch.1<\/strong> from the Design Manager. Sketch.1 is displayed in the Profiles box.<\/p>\n

Select Full revolve<\/strong> for Direction 1.<\/p>\n

Click OK<\/strong> (green checkmark) to complete the task.<\/p>\n

\"\"<\/p>\n

Display a Trimetric View.<\/p>\n

Click Trimetric View <\/strong>from the expansion arrow in the Work Area. Revolve.1 is created. Sketch.1 is fully defined.<\/p>\n

\"\"<\/p>\n

Note:<\/strong> To edit an existing feature, click the feature<\/strong> in the Design Manager, select Edit Feature<\/strong> in the Context toolbar.<\/p>\n

\"\"<\/p>\n

 <\/p>\n

Note<\/strong>: Click Undo<\/strong> or Redo<\/strong> in the Action bar to reverse or recover the last action.<\/p>\n

\"\"<\/p>\n

 <\/p>\n

Modify Sketch.1. Delete the top vertical line. Insert a 3 Point Arc.<\/p>\n

Insert a Tangent constraint.<\/p>\n

Right-Click Sketch.1<\/strong> in the Design Manager. The General tools are displayed.<\/p>\n

Click Edit Sketch<\/strong> in the Content toolbar.<\/p>\n

\"\"<\/p>\n

Display a Front view using the Triad.<\/p>\n

Click the yz face<\/strong> in the Triad as illustrated.<\/p>\n

\"\"<\/p>\n

Front view is displayed.<\/p>\n

\"\"<\/p>\n

Edit a Sketch<\/h2>\n

Delete the top vertical line.<\/p>\n

Click the top vertical line<\/strong>.<\/p>\n

Click Delete <\/strong>from the General drop-down Context box. Note<\/strong>: You can also press the Delete button.<\/p>\n

\"\"<\/p>\n

The Equal constraint remains on the two vertical lines maintaining design intent of the sketch.<\/p>\n

Delete the 20mm dimension.<\/p>\n

Click the 20 leader line<\/strong>.<\/p>\n

Click Delete <\/strong>from the General drop-down Context box.<\/p>\n

\"\"<\/p>\n

Apply the Three Point Arc Sketch entity.<\/p>\n

Click Three Point Arc<\/strong> from the Action bar.<\/p>\n

\"\"<\/p>\n

Click the first point<\/strong> as illustrated.<\/p>\n

Click the second point<\/strong> as illustrated.<\/p>\n

Click the third point<\/strong> as illustrated.<\/p>\n

\"\"<\/p>\n

Deactivate the Three Point Arc sketch entity.<\/p>\n

Press the Esc<\/strong> key.<\/p>\n

Insert two Tangent constraints between the vertical lines and the arc.<\/p>\n

Click the first point<\/strong>.<\/p>\n

Click Tangent <\/strong>from the Context box.<\/p>\n

\"\"<\/p>\n

Click the second point<\/strong>.<\/p>\n

Click Tangent<\/strong> from the Context box.<\/p>\n

\"\"<\/p>\n

Dimension the Arc.<\/p>\n

Click Sketch Dimension<\/strong> from the Action bar. View the Sketch Dimension icon.<\/p>\n

\"\"<\/p>\n

Click the Arc<\/strong>.<\/p>\n

Click a position<\/strong> above the Arc.<\/p>\n

Enter 10<\/strong>. The dimension displays R to indicate radius.<\/p>\n

Deactivate the Sketch Dimension.<\/p>\n

Press the Esc <\/strong>key.<\/p>\n

Accept the Sketch and exit.<\/p>\n

Click Accept Sketch<\/strong>.<\/p>\n

\"\"<\/p>\n

Display a Trimetric View.<\/p>\n

Click Trimetric View<\/strong> from the expanded arrow in the Work Area.<\/p>\n

\"\"<\/strong><\/p>\n

Sketch.1 is fully defined. The Revolved Pin component is finished.<\/p>\n

Save<\/strong> and Close<\/strong> the model.<\/p>\n

There are different techniques in xDesign to dimension a sketch.<\/p>\n

Option 1: As you sketch, the Dimension Edit Box is displayed. Click the sketch entity. Enter the dimension in the Dimension Edit Box.<\/p>\n

Option 2: Click the sketch entity. Click Distance from the Context toolbar. Enter the distance. This constrains the distance between the selected entities.<\/p>\n

Option 3: Click Sketch Dimension in the Action bar. Click the sketch entity. Click a position to enter the dimension. Enter the dimension. This option provides the ability to place and move the dimension.<\/p>\n

 <\/p>\n

Academic Community:<\/strong> After you create a 3D<\/strong>EXPERIENCE ID, Educators, can get more information on xDesign and SOLIDWORKS.\u00a0 Request to join the 3D<\/strong>EXPERIENCE Academic Community for free at go.3ds.com\/academiccommunity.<\/p>\n

Student Community:<\/strong> Students, join the student community for free at go.3ds.com\/studentcommunity.\u00a0 Check out great posts on Mechanism Mondays, FEA Fridays, \u00a0Solid Saturdays (animations),\u00a0 Formula Student and Formula SAE exercises.<\/p>\n

Stay tuned for David’s next SOLIDWORKS xDesign Lesson #11: \u00a0Features <\/strong><\/p>\n

To review the previous lessons, go to:<\/p>\n

SOLIDWORKS xDesign Lesson #1: Getting Started<\/strong><\/a><\/p>\n

SOLIDWORKS xDesign Lesson #2: Mouse Control and Collaborative Space<\/strong><\/a><\/p>\n

SOLIDWORKS xDesign Lesson #3: Sketch Planes<\/strong><\/a><\/p>\n

SOLIDWORKS xDesign Lesson #4: Create A Dashboard<\/strong><\/a><\/p>\n

SOLIDWORKS xDesign Lesson #5: Views and Orientations<\/strong><\/a><\/p>\n

SOLIDWORKS xDesign Lesson #6: Importing Files and Using Bookmarks<\/strong><\/a><\/p>\n

SOLIDWORKS xDesign Lesson #7: Assemblies<\/strong><\/a><\/p>\n

SOLIDWORKS xDesign Lesson #8: 4Bar Linkage and Kinematics<\/strong><\/a><\/p>\n

SOLIDWORKS xDesign Lesson #9: External References and Copy with Mates<\/a><\/strong><\/p>\n

\u00a0<\/strong><\/p>\n","protected":false},"excerpt":{"rendered":"

Design intent manages the relationship between sketches in a feature, features in a part, and parts in an assembly. Students need to understand design intent in a sketch, using constraints and dimensions. Let’s start with a simple example using xDesign.<\/p>\n... Continued<\/a>","protected":false},"author":84,"featured_media":14737,"comment_status":"open","ping_status":"closed","sticky":false,"template":"","format":"standard","meta":{"_acf_changed":false,"footnotes":""},"categories":[6862,7233,5381,4184,4183,5204,6712,4015,5205,5211],"tags":[7060,7059,5281,6973,7232,4460,4631,6956,4146,3931,7223,6637,7171,4318,6392],"class_list":["post-14734","post","type-post","status-publish","format-standard","has-post-thumbnail","hentry","category-3dexperience","category-3dexperience-works","category-cad-2","category-cad-instructor","category-cad-teacher","category-curriculum-2","category-education","category-mechanical-engineering","category-stem-course","category-technology-2","tag-3dexperience-works","tag-3dexperienceworks","tag-3dexperience","tag-cloud-cad","tag-constraints","tag-dimensions","tag-educators","tag-features","tag-sketch","tag-solidworks","tag-solidworks-cloud-cad-apps","tag-solidworks-xdesign","tag-solidworksxdesignlesson","tag-tutorials","tag-xdesign"],"acf":[],"_links":{"self":[{"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/posts\/14734","targetHints":{"allow":["GET"]}}],"collection":[{"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/posts"}],"about":[{"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/types\/post"}],"author":[{"embeddable":true,"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/users\/84"}],"replies":[{"embeddable":true,"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/comments?post=14734"}],"version-history":[{"count":17,"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/posts\/14734\/revisions"}],"predecessor-version":[{"id":14899,"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/posts\/14734\/revisions\/14899"}],"wp:featuredmedia":[{"embeddable":true,"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/media\/14737"}],"wp:attachment":[{"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/media?parent=14734"}],"wp:term":[{"taxonomy":"category","embeddable":true,"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/categories?post=14734"},{"taxonomy":"post_tag","embeddable":true,"href":"https:\/\/blogs.solidworks.com\/teacher\/wp-json\/wp\/v2\/tags?post=14734"}],"curies":[{"name":"wp","href":"https:\/\/api.w.org\/{rel}","templated":true}]}}