Putting a lip on an angle in sheet advisor

[Jim Kuchar]

Take a .030 thick by .50 wide by 10 in. longpiece of sheet metal. Cut an angle on top at say 30 degrees. How do you add a lip onto the angled edge? I tried the add lip command in sheet advisor and it gives me an error. If I offset the edge during the lip command I can fudge the detail but this is not what I want in the part. The manufacturing process would be to put the strip of metal in a sheet metal brake. Turn the sheet metal at a 30 degree angle and bend it up 90 degrees. How do I create this detail in solid designer?

[Jack Dannenberg]

Hi Jim, This particular case must be done with a workplane and a profile. Put the workplane on the angular face and create a profile to give the desired lip height. Now is the critical part. The system can see that the sides of the part are not at 90 degrees to the WP so it will add bend reliefs. On the short edge of the part the relief will go into the interior of the part. But on the long side the relief would break out of the part. Therefore you need to move the vertical side of the profile in towards the other vertical side, i.e. make the profile narrower. Because you do not want the lip to be narrower you you modify the shape as below. Sorry, Microsoft says I canot use vertical bars in an email message, so no picture. You move the short vertical segment in far enough so that the bend relief will not break through the side of the part. Naturally a picture is worth a thousand words. Email me and I will send you a jpeg of the part, WP and profile and it will probably much easier to understand.

[Mario Fischer]

Hi Jim, here are some good news: in SheetAdvisor 8.0 you will be able to easily create those lips with the Add Lip command. For the time being you can use Jack's solution or use the fold/unfold command. To use the fold/unfold command some addtional work is necessary. First you need to extend your part. That is lift the face that you want to attach the lip to (in Modify 3D - Faces - Lift). Just use some value to lift the face and later adjust the face by either using lift agian or move faces. Now you need to imprint the bend zone. This is the tricky part. Create a workplane parallel to the top face of your part. Create a construction line where the lifted face has been. Create a further construction line parallel to this towards the existing part by a distance of d+ri (thickness + inner radius of the bend). This line is the starting line of your bend. Now you need to know the bend length, ie. the length of the bend when it is unfolded. The formula for this is l = (ri + k*d) * phi, where l - bend length, ri - inner radius of the bend; k - k-factor for bend/marterial; d - thickness of material; phi - bend angle. If you do not know the k-factor or don't want to bother the formula you can just create a bend with the same parameters, unfold it (using fold/unfold) and measure the bend length. Use this length to create a third line with a distance of l to the second bend line. These two lines define the bend area. Create a polygon and imprint the polygon to the part (Machine - imprint edges - linear). Now you can use the fold/unfold command to create the bend. Last step is to adjust the lip length. The next version of SheetAdvisor will allow you to easily create a bend from the flat. Send me an Email if you have problems or if something isn't clear. As Jack said a picture is worth a thousand words. Guess it would help here, too. Mario