I am messing around with a part at the moment so if I was to put it up as an .ipt file it would be crucified for not being constrained, dimensioned etc etc.
I am stumped I have to say. I am trying to get a 25 and 20mm return fold on the back of a curved panel. No matter what I have tried I cannot figure out how to do this, I manged to get the model bend on it however this will not flatten out in Sheet metal correctly and I will need to send a drawing out in a flattened state.
The folds needed are shown in picture as well as the curved part
They need to go on the outer bend of the plate. If I tell the mmanufacturers to weld it in points along the flange that's ok, I just can't seem to model it to get a final drawing out!
Go on, you guys are gonna say its ...blah blah...click this its done...I just know it
Solved! Go to Solution.
I manged to get the model bend ....
Bend does not sound right. You should not use Inventor Bend Part feature for this.
(worry about the holes later)
Or put the entire single line profile in one sketch and Contoured Flange. (Inventor will add the bends.)
Attach you attempt here.
Ahh i am sorry I wasnt very good with my explanation.
The fold is coming off the top outer edge, my mistake i should have said.
ok, I see where I have gone wrong
I can now get the rolled edge. I cannot get the holes, if I flat part then 2D sketch, I get a message saying only edits in flat part will be done not in a folded.
I am working on the radius generated from Chord length and Median line to discover the radius. I cannot get the rolled part to achieve the correct length I need , the only adjust I can make is the rolled angle, which I do not know.
I know the distance of the outside edge, and the chord distance from each end of the arc.
Maybe I am reading or trying to do more than Inventor can do?
In the Contour Roll dialog box, change the Unroll Method to Developed Length and then enter the Length you want to end up with.
Then use the Unfold tool (not the Create Flat Pattern tool) to temporarily unfold the part. Then sketch one of your slots, and use the Cut tool to create it. Then use the Rectangular Pattern tool to place the rest of the slots. And finally, use the Refold tool to set the part back to it's correct folded condition.
Now you can generate your flat pattern, and the length should be correct.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
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Thanks guys, does the dveloped length keep the radius as that is crucial too? Its basically a curved guard that fits to a conveyor that curves through 90 deg.
the curve required is not through the full 90 deg but a portion of it, so curvature, developed length and radius are very important as its being made from 3mm steel and will be difficult to manipulate.
Its late, so I will give this a go over the next few days, but I've learnt loads just in one night...thank you!
Will post if i get it correct
Thanks guys, All the help has concluded to this. Finally after a lot of twiddling the result!
Couldnt have got this with out you all
An old subject but I found the solution I was looking for however when the flange is reversed the model and the flat sheet are not correct.
Please see the attached phtographs fo the actual fabricated panels. These show to reverse the information in the flat sheet drawings is no correct - the v cuts are neededflange we need to make V-Cuts in the flange to allow this to be bent in the reverse direction and folded. My question is can Inventor undertake this?
We have had sisues where the fabricators are undertaking the final fabricated aluminium panels incorrect in accoerdance witht he required geometry and they are struggling to create the drawings. We have therfore, only this week, looked at Inventor as a source to assist in this - we can model the panels but the flat sheet is not correct and does not show the required V-Cuts to create a reversed flange - like the images.
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