WF - Sheetmetal Q

: "CKERIDES" wrote : Have a simple "L" shaped part created as an extruded wall and can not add a : flat wall to any of the edges. No problems adding a flat wall w/ a radius but : not a flat wall w/ no radius -

There are so many ways that one can do this incorrectly that I'd like to go over some basics. First some cautions.

• Accuracy considerations play a prominent role in sheet metal because you automatically have a high ratio between thin sheet thickness and overall part size, especially true if you include non-zero inside radiuses that are a fraction of part thickness, a common technique for avoid interference at corners. Setting the accuracy ratio as high as it will go, then easing it down, regenerating until it fails, is a good way to find what the accuracy value will sustain. Then you move the decimal point one place to the left and regenerate. But start out high and go down to find out what it will tolerate. Right from the start, you want to rule out Pro/GOOFY's accuracy value as a cause of your troubles.

• Extruded features of more than one "wall" or bend, as a FIRST WALL, make their own difficulties. For one, with an angle like yours, it will not form an inside radius as it can when you produce the wall separately. If you wish an inside radius, you have to include it in the sketch. If you wish a nominal, very small inside radius, this becomes a problem.

• If you sketch two lines at right angles, as your description suggested, you can, by putting the material direction to the inside of the bend, create an impossible sheetmetal part ~ both the outside and inside radiuses will be sharp. Pro/e may be able to make such a "bend" but this won't give you an accurate developed length. And you can't get such a part out of a stamping press.

Did you attach your flat wall to an inside edge? If you did and you sketched the flat wall to the inside of the bend, it should have worked fine, even with a zero radius attachment. If you attached the sketch to the outside edge and sketched to the inside (crossing wall thickness), the flat wall will try to maintain on a plane with the end of the angle wall. The ouside of your flat wall will be even with the end of the angle wall. That means that, at the corner, you need rip relief, at least as much as the outside radius, because the bend goes *into* the attachment wall and "eats up" part of it. If the outside corner happened to be sharp, the end of the angle wall would interfere with corner relief and would fail. In any case, I advocate against *any* zero inside corners: they don't exist, the dies always get "dressed", sharp corners are broken to keep the bending operation from shearing off a tab, the shorter the tab, the greater the tendency to shear and break. But this slight deviation from nominal sharp also makes attached flat walls less likely to fail because of interference in the corner.

David Janes

Added a radius to the sketched "L" shape and got the flat wall w/ no rad to regenerate fine- Is there a way to dimension OD/OD of a sketched "L" shape that is not 90 degs? In other words, the "L" shape bracket I have has one sketched line at zero and the other at 80 degs so when I add the rad the OD dimensions switch to tangent pts on the rad -

Maybe you need to flip the material direction to the inside of the sketched curve. Then the sketch will be the outside of the part. Or, maybe I need pictures. I'm spoiled by looking at a tube where I can see (though not necessarily describe) problems. I think Pro/e is easy; describing problems I'm having to people who are not looking at my tube is the really hard part.

David Janes

If I flip the mat'l I'll still have a radius just a mat thickness smaller - Try this as an extruded wall: sketch two lines one inch in length each. One line is horizontal and the other extending from the horizontal line but at 80 degs - Now add a radius - Although I believe the actual length of the flanges remain at one inch each, the dimension scheme changes from end pt to end pt TO end pt to tangent pt of rad/other when the radius is added - Is there a way to dimension the flanges at one inch each regardless of the radius size?

: "CKERIDES" wrote : >

: >Maybe you need to flip the material direction to the inside of the sketched : >curve. : >Then the sketch will be the outside of the part. Or, maybe I need pictures : : If I flip the mat'l I'll still have a radius just a mat thickness smaller - Try : this as an extruded wall: sketch two lines one inch in length each. One line is : horizontal and the other extending from the horizontal line but at 80 degs - : Now add a radius - Although I believe the actual length of the flanges remain : at one inch each, the dimension scheme changes from end pt to end pt TO end pt : to tangent pt of rad/other when the radius is added - Is there a way to : dimension the flanges at one inch each regardless of the radius size? : Here's the problem with extruded walls: they'll only dimension the way the sketch was dimensioned. If you can figure out how to dimension to sharp corners in the sketch, it will show up that way in the drawing. But only to the sketched profile ~ this can turn into the inside or outside surface of the sheetmetal part. You may even put the sketch down the midplane of the part. But ANY of these will not accuractely reflect your develped length. This leaves me in doubt as to what use it will be but that's your business.

David Janes

Modeled up a few sheetmetal parts based from 2D drawings that did not show the rad's - In order to check the OD dimensions had to create them in a drawing as opposed to sketching them The sheetmetal company requires OD/OD dimensions (apex to apex) to form the flange lengths and they use their own unfolding software to get the flat patterns - It would be nice to be able to show the dimensions in a drawing instead of creating them, but my main reason for asking the question is that I find it surprising that you can't add a flat wall w/ no rad to an extruded wall unless it has a radius and since that's the case, there should be a way to "sketch" OD/OD dimensions at any angle

FYI "Add a point at the intersection. Then dimension flange from edge to point." This works-