Problem - Can anone help

I have a problem, and i would appreciate some help. Here is the
situation.
1. I have to model a 150x25 channel rolled to 2000id, toes out. The way
i did this was to insert the appropriate sketch from the structural
steel toolbox and then, with the help of a centre line, used the
revolve boss command to complete.
2. Now i have put holes to put on the inside face. I cannot think of an
easy way of doing this. Maybe I have drawn the channel wrong in the
first instance. I would prefer to be able to flatten the channel, but
using the revolved boss command has made this impossible.
Any help would be much appreciated!
Reply to
nigel.rafferty
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I would suggest creating a long straight channel of the proper length, adding all of your holes, and finally bending the piece with the Flex command.
Alternatively, you can create the the revolved part, create the sketch for your holes, and perform a Wrap operation to cut the holes. (This was suggested by P. in a previous posting.)
Depending upon your goal, you might consider simply cutting circular holes in the revolved part. Although this won't accurately represent the finished part (assuming the holes are to be drilled prior to bending), it would be convenient for dimensioning in a drawing.
You mentioned flattening the channel after creating it with a revolve. You would have to make the channel a sheetmetal part in order to take such an approach. Such an approach is possible, but would require you to change the channel to be a sheetmetal part with constant wall thickness, etc. I assume you will be happier with an approach that would avoid this restriction and allow you to accurately represent the structural steel profile.
Reply to
John Eric Voltin
Wrap has the advantage of providing dimensions from the sketch in the drawing.
John Eric Volt> I would suggest creating a long straight channel of the proper length,
sketch for
revolve. You
restriction and
Reply to
P.
Good point. I hadn't thought of that.
Reply to
John Eric Voltin
2 other possibilities- A)draw a revolved hole somewhere using a new radial plane and use the circular pattern tool and your axis of rotation to generate your other holes- suppress any unwanted instances B)use the hole wizard to pick 3d points on the surface
Reply to
neil
possibility 3 make a flat web and insert a bend, flatten bend ,cut in your holes, rebend and revolve or sweep some flanges onto it, add fillets. this will allow you to produce a flattened view of the flange back with holes shown in a dwg
Reply to
neilscad
actually I take back no.3 because interestingly if you flatten the part after adding the flanges the sheetmetal has been trimmed by them....hmmm...I thought this used to work this way....oh well
Reply to
neil
haha!! ...it does work after all...suppress the flange features when you make the dwg flat pattern....enough posts all ready - gotta get away from this pc for a while..perils of being self employed.
Reply to
neil
Well, I didn't think of it either till he asked and I did some testing. I've been trying to find a way to get holes on curved surfaces that I can dimension on a print. Finding the answer to his question helped a bit in that direction.
John Eric Volt> Good point. I hadn't thought of that.
circular
structural
channel,
Reply to
P.
Thanks everyone!!!!
Reply to
nigel.rafferty

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