{"id":133219,"date":"2021-08-27T21:50:00","date_gmt":"2021-08-28T01:50:00","guid":{"rendered":"https:\/\/live-cati-marketing.pantheonsite.io\/solidworks-using-pattern-driven-component-patterns\/"},"modified":"2022-04-20T19:01:46","modified_gmt":"2022-04-20T23:01:46","slug":"solidworks-using-pattern-driven-component-patterns","status":"publish","type":"post","link":"https:\/\/www.cati.com\/?p=133219","title":{"rendered":"SOLIDWORKS: Using Pattern Driven Component Patterns"},"content":{"rendered":"<p>Recognizing symmetry or repetition in our designs can be indication that we can save significant modeling time by capturing our design intent. In our <a href=\"https:\/\/www.cati.com\/3d-cad\/solidworks-3d-cad\/\">SOLIDWORKS<\/a> assemblies, we have a very powerful command called \u201c<strong>Pattern Driven Component Pattern<\/strong>\u201d. With this command, you can pattern components in your assembly based on pattern features that exist in your part files. If the feature pattern is adjusted in the part file, the patterned components will adjust to match in your assembly file. This is a great way to capture your design intent and make sure things match. This usage of <strong>Pattern Driven Component Pattern<\/strong> command is covered in detail in an earlier <a href=\"https:\/\/www.cati.com\/blog\/2019\/07\/solidworks-assembly-patterns-using-pattern-driven-components\/\">blog post<\/a>.<\/p>\r\n<p>What I wanted to show today, is another way to use this command even if the part did not actually have a pattern feature. This exception is based on part geometry created with the Hole Wizard command.\u00a0 It can be an excellent time saver for tasks like putting fasteners in holes.<\/p>\r\n<p>Let\u2019s look at a SOLIDWORKS assembly where we would like to add several fasteners to hold it together.<\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86523\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/a-picture-containing-logo-description-automatical-1.png\" alt=\"A picture containing logo\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>Let\u2019s start by creating the screw holes in the outer blue part. For this operation, we will use the <strong>SOLIDWORKS Hole Wizard<\/strong> feature. To take full advantage of the <strong>Pattern Driven Component<\/strong> <strong>Pattern<\/strong> command, we want to create the holes in a single <strong>Hole Wizard<\/strong> feature.<\/p>\r\n<p>After identifying the Socket-Head Cap Screw as the type of hole geometry we need, we switch to the \u201cPositions\u201d tab. To place holes on multiple faces of the part, we use the \u201c3D Sketch\u201d button.<\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86524\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/graphical-user-interface-text-application-descr-29.png\" alt=\"Graphical user interface, text, application\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>Inside this 3D Sketch, we can place sketch points to locate our holes.<\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86525\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/diagram-description-automatically-generated-10.png\" alt=\"Diagram\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>Mirroring these sketch points, inside this 3D sketch, can save us some additional time.<\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86526\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/chart-description-automatically-generated-10.png\" alt=\"Chart\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>After completing the single <strong>Hole Wizard<\/strong> feature, we now have all twelve desired holes in the part model.<\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86527\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/icon-description-automatically-generated-7.png\" alt=\"Icon\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>Now, let\u2019s jump back to the assembly file. We insert the initial instance of a socket head cap screw, washer, and nut.<\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86528\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/a-picture-containing-text-description-automatical-5.png\" alt=\"A picture containing text\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>Now, we want to add several of these fastener combinations. We need one for each of these twelve bolt holes. The command we will use is <strong>Pattern Driven Component Pattern.<\/strong><\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86529\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/graphical-user-interface-text-application-descr-30.png\" alt=\"Graphical user interface, text, application\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>For the \u201cComponents to Pattern\u201d, we select the nut, bolt, and washer. For the \u201cDriving Feature\u201d we select the <strong>Hole Wizard<\/strong> feature from the part file.<\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86530\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/diagram-description-automatically-generated-11.png\" alt=\"Diagram\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>Mission accomplished! We have fasteners in all our bolt holes.<\/p>\r\n<p><img decoding=\"async\" class=\"wp-image-86531\" src=\"https:\/\/www.cati.com\/wp-content\/uploads\/2021\/08\/a-picture-containing-diagram-description-automati-2.png\" alt=\"A picture containing diagram\r\n\r\nDescription automatically generated\" \/><\/p>\r\n<p>As you can see, this is a time saver and captures our design intent of fasteners in every bolt hole in the part file. If we edit the <strong>Hole Wizard<\/strong> hole quantity or placement, these assembly fasteners will update to match. Hopefully, this gives you additional appreciation for the very useful <strong>Pattern Driven Component Pattern<\/strong> tool in <strong>SOLIDWORKS<\/strong>.<\/p>\r\n\r\n<p class=\"wp-block-paragraph\">Greg Buter<br \/>Application Engineer Manager<br \/><a href=\"http:\/\/www.cati.com\/\">Computer Aided Technology<\/a><\/p>\r\n","protected":false},"excerpt":{"rendered":"<p>Recognizing symmetry or repetition in our designs can be indication that we can save significant modeling time by capturing our design intent. In our SOLIDWORKS assemblies, we have a very powerful command called \u201cPattern Driven Component Pattern\u201d. With this command, you can pattern components in your assembly based on pattern features that exist in your [&hellip;]<\/p>\n","protected":false},"author":31,"featured_media":133220,"comment_status":"open","ping_status":"open","sticky":false,"template":"","format":"standard","meta":{"_acf_changed":false,"footnotes":""},"categories":[1085,1086,1307,1090,1094,1099],"tags":[],"class_list":["post-133219","post","type-post","status-publish","format-standard","has-post-thumbnail","hentry","category-design-engineering","category-solidworks-3d-cad","category-photoview-360","category-technical-communication","category-announcements","category-solidworks-whats-new"],"acf":[],"yoast_head":"<!-- This site is optimized with the Yoast SEO Premium plugin v22.5 (Yoast SEO v22.5) - https:\/\/yoast.com\/wordpress\/plugins\/seo\/ -->\n<title>SOLIDWORKS: Using Pattern Driven Component Patterns<\/title>\n<meta name=\"description\" content=\"The \u201cPattern Driven Component Pattern\u201d command in 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