{"id":17131,"date":"2017-06-09T17:00:45","date_gmt":"2017-06-09T21:00:45","guid":{"rendered":"https:\/\/blogs.solidworks.com\/tech\/?p=17131"},"modified":"2017-06-09T09:45:05","modified_gmt":"2017-06-09T13:45:05","slug":"solidworks-modeling-challenge-measuring-imported-fillets","status":"publish","type":"post","link":"https:\/\/blogs.solidworks.com\/tech\/2017\/06\/solidworks-modeling-challenge-measuring-imported-fillets.html","title":{"rendered":"SOLIDWORKS Modeling Challenge – Measuring Imported Fillets"},"content":{"rendered":"

* This is one of a series of <\/span><\/i>modeling challenges<\/span><\/i><\/a> you can use to test your SOLIDWORKS skills. \u00a0First, read the challenge and try to figure out a solution on your own. \u00a0Then, compare your solution with my good, better, and best recommendations. \u00a0As always, feel free to share even more tips and tricks in the comments below.<\/span><\/i><\/span><\/p>\n

Modeling, measuring, and modifying native SOLIDWORKS files is easy. \u00a0Most of the really fun modeling challenges arise when working with imported geometry. \u00a0All you\u2019re typically given to start off with is what we call a \u201cdumb solid\u201d – just a hunk of digital mass with no intelligence (i.e. parametric feature history). \u00a0Sometimes you\u2019re even left at the mercy of another CAD system\u2019s inferior export quality. \u00a0This can be troublesome, because what one CAD system may consider cylindrical, SOLIDWORKS may not.<\/span><\/p>\n

For example, imagine importing what looks like a simple sheet metal part file, using the Convert to Sheet Metal tool to flatten it, and then realizing it won\u2019t work because the bent faces aren\u2019t perfectly cylindrical. \u00a0The only workaround is to replace the filleted faces with true cylindrical faces. \u00a0Here\u2019s how to do it:<\/span><\/p>\n

\"\"<\/p>\n

    \n
  1. Use Copy Surface (<\/span>Offset Surface<\/span><\/a> with an offset value of 0) to copy the flat faces<\/span><\/li>\n
  2. Use <\/span>Delete Body<\/span><\/a> to delete the original imported solid<\/span>
    \n<\/span>Expand the solid body folder, select the body, and click the delete key to quickly activate this tool<\/span><\/i><\/span><\/li>\n
  3. Use <\/span>Extend Surface<\/span><\/a> to fill the gaps of the removed filleted faces<\/span><\/li>\n
  4. Use <\/span>Face Fillet<\/span><\/a> to bridge between the surface bodies with a perfectly tangent transition<\/span><\/li>\n
  5. Use <\/span>Convert to Sheet Metal<\/span><\/a> to convert the surface body to a sheet metal solid body<\/span><\/li>\n
  6. Now you can use the <\/span>Flatten<\/span><\/a> command to display the flat pattern<\/span><\/li>\n<\/ol>\n

    So that\u2019s a pretty cool tip, but that\u2019s not the modeling challenge for this post. \u00a0I skipped a step between #3 and #4. \u00a0First you need to know the size of the fillet before you can model it. \u00a0Since imported models don\u2019t have feature dimensions, the challenge is – how do we measure imported fillets?<\/span><\/p>\n

    Status Bar<\/b><\/h1>\n

    Most of us know you can use the Status Bar (the informational text shown in the bottom right hand corner of the SOLIDWORKS interface) to display measurements of select edges and faces. \u00a0Most of us also know if you select a circular edge, the Status Bar will report a radius. \u00a0This can help in situations as shown on the left end of the model below. \u00a0The problem is that when selecting an edge that isn\u2019t perfectly normal to the direction of the circular profile, all the Status Bar will report is an Arc Length – no help when trying to measure a fillet. \u00a0So what do we do when neither edge of a cylindrical face is normal to the profile of the fillet? \u00a0SOLIDWORKS solved this problem in 2015 when we added the <\/span>ability to display a radius value when selecting a cylindrical face<\/span><\/a>. \u00a0It\u2019s a pretty simple solution that you definitely want to be aware of!<\/span><\/p>\n

    \"\"<\/p>\n

    Normal Profile Sketch<\/b><\/h1>\n

    The last solution works for cylindrical faces, but what about fillets that are applied to a curved edge (i.e. fillets that aren\u2019t cylindrical)? \u00a0In these cases, we\u2019ll need to create a circular profile to measure. \u00a0Here\u2019s an easy way to do so:<\/span><\/p>\n

    \"\"<\/p>\n

      \n
    1. Select the vertex and the edge of the fillet and then create a sketch<\/span>
      \n<\/span>By preselecting a vertex and an edge before creating a sketch, SOLIDWORKS automatically generates a plane coincident to the vertex and normal to the edge and activates a new sketch on that plane all in a single step<\/span><\/i><\/span><\/li>\n
    2. Select the filleted face and then create an <\/span>Intersection Curve<\/span>
      \n<\/span><\/a>And Intersection Curve will generate a sketch entity at the intersection of the selected face and the active sketch plane which will create a circular arc normal to the profile of the fillet<\/span><\/i><\/span><\/li>\n
    3. Select the resultant arc to display the measured radius in the Status Bar<\/span><\/li>\n<\/ol>\n

      Curvature Evaluation<\/b><\/h1>\n

      Even with those nifty shortcuts, that last tip still took too many steps for me. \u00a0It also wouldn’t have helped us with our original imported sheet metal example that didn\u2019t contain fillets with exact radii. \u00a0That leads us to our final solution. \u00a0It\u2019s actually way too easy, but it\u2019s also commonly overlooked and neglected, which is why I felt compelled to write this post. \u00a0To measure any fillet in any condition, all you have to do it fire up the <\/span>Curvature Evaluation<\/span><\/a> tool and hover over the filleted face. \u00a0SOLIDWORKS will <\/span>display a live measurement of the curvature<\/span><\/a> directly under your mouse. \u00a0That\u2019s all there is to it!<\/span><\/p>\n

      \"\"<\/p>\n

      If you create models with a ton of different sized fillets, this is also a great way to make a quick final inspection to make sure all of your fillets were applied correctly. \u00a0Enjoy!<\/span><\/p>\n","protected":false},"excerpt":{"rendered":"

      * This is one of a series of modeling challenges you can use to test your SOLIDWORKS skills. \u00a0First, read the challenge and try to figure out a solution on your own. \u00a0Then, compare your solution with my good, better,<\/p>\n... Continued<\/a>","protected":false},"author":193,"featured_media":17132,"comment_status":"open","ping_status":"closed","sticky":false,"template":"","format":"standard","meta":{"_acf_changed":false,"footnotes":""},"categories":[1709,35,36],"tags":[1971,1972,880,1129,1970,1969],"class_list":["post-17131","post","type-post","status-publish","format-standard","has-post-thumbnail","hentry","category-modelingchallenge","category-tips-tricks","category-usability","tag-curvature-evaluation","tag-measuring-imported-fillets","tag-modeling-challenge","tag-modeling_challenge","tag-normal-profile-sketch","tag-status-bar"],"acf":[],"_links":{"self":[{"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/posts\/17131","targetHints":{"allow":["GET"]}}],"collection":[{"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/posts"}],"about":[{"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/types\/post"}],"author":[{"embeddable":true,"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/users\/193"}],"replies":[{"embeddable":true,"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/comments?post=17131"}],"version-history":[{"count":5,"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/posts\/17131\/revisions"}],"predecessor-version":[{"id":17139,"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/posts\/17131\/revisions\/17139"}],"wp:featuredmedia":[{"embeddable":true,"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/media\/17132"}],"wp:attachment":[{"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/media?parent=17131"}],"wp:term":[{"taxonomy":"category","embeddable":true,"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/categories?post=17131"},{"taxonomy":"post_tag","embeddable":true,"href":"https:\/\/blogs.solidworks.com\/tech\/wp-json\/wp\/v2\/tags?post=17131"}],"curies":[{"name":"wp","href":"https:\/\/api.w.org\/{rel}","templated":true}]}}