is there I a way for me to flatten a part after I've created a knit and feature from a face that is curved? I can't figure it out. The part has a arc with no flat areas for me to select a face or an edge.
Could you attach the part so we can take a look at it?.. I do not have flatten surfaces capability with professional, but might be able to do it with the sheet metal tools.
here is the attachment. Any help is much appreciated! We are trying to convert this shape into a flat pattern so that it becomes a graphic decal.
Carlos,, you are going to get a kick out of this. I don't understand why what you had didn't work. I suspect you put that boss extrude (tab) in there in order to have a flat face for inserting bends. I tried putting a tab on the end of the part (since I believe this works in one direction only) but couldn't get that to work. I eventually did a base flange off an arc (with a tangent line on the end) then cut the part up. All your stuff is in the part (hidden) and you can see it all lines up. I have some failed stuff in there also just suppressed it. You can alter the tab on the end in order to make it less obvious. It does flatten correctly. I have attached a 2015 file. Looks like that is what you are using. This was definitely a challenge.
I found this in the SolidWorks Help files. Note the highlighted sentence. It looks like the holes are the problem for "Surface Flatten".
Thanks Andy for your reply. However, the method i used to create the shape with knit and thicken. In doing so, the holes come along. Is there a way to eliminate the hole cutouts when do the knit and thicken?
Andy, I tried the method you are suggesting, but I'm having difficulties. I tried creating a solid surface, but the surface flatten icon stays grayed out. The Knit face and thicken command also keeps the surface flatten icon grayed out. What steps do I need to follow in order to make this operation a success?
You cannot use the Surface Flatten command on a solid body. First you need to select the face of your solid body & use the Offset Surface command on the Surface tab, set it to "0". Hide the solid body, then Ctrl select the edges of the holes on the surface body & press delete on your keyboard & remove the holes. Then you should be able to use the flatten surface command giving the required inputs.
SolidWorks 2016 allows you to flatten surfaces with holes & internal geometry now, as long as you have the premium version I think.
Carlos,.. I did a insert/part and added a tab... plus.. "I had to" add radii at the tab for it to work..
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