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looking for another method of cleaning a file


ezra

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Hello All,

I have problems sometimes with sketches having open sections, or shared points, in general, I would call the geometry unpure, and unsuitable for extrusion. I am wondering if there is a way to clean up a file faster than increasing the zoom on sections and visually inspecting them, does Solidworks have a way of pointing out impurities in a sketch?

I will appreciate any information passed on to me.

 

 

Ezra

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What version of Solidworks are you running?

 

Yes there are tools in the sketch environment that help you find open sections and issues. If you go to the Tools Menu(in 2016 SW changed the menu structure fyi) there are two things that might be of interest to you. Tools >Sketch Tools > Repair Sketch and Tools > Sketch Tools > Check Sketch for Feature.

 

When you use Repair Sketch you enter a gap value and it will automatically find them and turn on the magnifying glass(G shortcut key).

 

When you use Check Sketch for Feature it lets you pick what feature you want to use(extrude for example) and "Check". If there is an issue it will tell you and ask you to try and fix it. The Fix will open up repair sketch.

 

Some other tips. Box selecting from the top left to bottom right will only select entities that are completely in the box. This helps if you have the little dangling sketch entities that happen from time to time. In newer versions of SW there is a "Shaded sketch contours" option on the toolbar that is handy to give you a quick preview of your sketch and if its actually closed. If you have two ends that overlap it won't count it as closed unless there are intersecting points.

 

If you have a specific example i an maybe give you a more specific answer but hopefully that helps.

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Thank you Mr Shift,

You have been a big help. Ironically I am using 2016-2017.

 

 

Ezra

 

 

 

 

 

 

What version of Solidworks are you running?

 

Yes there are tools in the sketch environment that help you find open sections and issues. If you go to the Tools Menu(in 2016 SW changed the menu structure fyi) there are two things that might be of interest to you. Tools >Sketch Tools > Repair Sketch and Tools > Sketch Tools > Check Sketch for Feature.

 

When you use Repair Sketch you enter a gap value and it will automatically find them and turn on the magnifying glass(G shortcut key).

 

When you use Check Sketch for Feature it lets you pick what feature you want to use(extrude for example) and "Check". If there is an issue it will tell you and ask you to try and fix it. The Fix will open up repair sketch.

 

Some other tips. Box selecting from the top left to bottom right will only select entities that are completely in the box. This helps if you have the little dangling sketch entities that happen from time to time. In newer versions of SW there is a "Shaded sketch contours" option on the toolbar that is handy to give you a quick preview of your sketch and if its actually closed. If you have two ends that overlap it won't count it as closed unless there are intersecting points.

 

If you have a specific example i an maybe give you a more specific answer but hopefully that helps.

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You are very welcome Ezra. If you come across an older version of solidworks the tools are still there but in 2016 they just made a shift in how the menus are organized is all. I have used a lot of CAD programs and the sketching in Solidworks is still my preference but others are catching up, but it can be very frustrating when a sketch doesn't work right! Also note in the Feature Manager that there are several changes to Icons and information about the sketch. For example if you see a (-) after a sketch name it means that it is under defined. So you need more dimensions or constraints. If you see a (+) it means its over defined. Very rare but can happen. a (?) means its missing a reference and you typically see that when a part is designed in context of an assembly and then opened by itself. There is also a different sketch icon that is sometimes called the "dead fish" that displays when you have multiple contours. Not a bad thing really but just a quick way to look at the feature tree and see these types of things.

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