Is it possible to modify this part so I can fold it out?

[Anonymous]

I have this part with a twisted middle. We figured out a solution yesterday where you weld it together but my boss wants it all in one piece. Is it possible to modify it somehow to unfold it? 

This attachment is not the prettiest and the work done on it is rough but you get the picture. 

[sam_m]

Is this any help?  (2014 format)

to enable it to unfold you need to make sure each fold is only in 1 direction (no plastic deformation) and to make sure the thickness is kept constant.  This wasn't true with your model as you have the plate 3mm thick with a 1mm fillet on 1 side but 2mm the other (1mm inside fillet + 3mm thickness doesn't equal 2mm outside fillet).

The easiest way I know to ensure everything is kept constant is to use surfaces to create 1 side of the part and then thicken the entire shape to give you the solid model.  Trying to keep the part as a solid, with the 3mm thickness, leads to headaches of small wedges of material left over here and there, and thus I try to avoid.

How I did your part:

used thicken with 0 distance to give me the inside face of the part and used the existing delete face command to remove the entire solid void to clean everything away.

I then removed the "dodgy" middle bit, to clean away the plastic deformed area.

Instead of a 90 degree upright and another 90 degree bend, like your go, I thought a diagonal is probably more representative of the original part, so I created a flat plate between the 2 sides and trimmed it down to suit.  Stiched it all together, added fillets and then thickened.  Robert's your mother's brother and all that jazz.  I hope it helps...

*edit* Also, next time, please don't create a new topic - just keep the posts going in the original one, as it helps keep the history of the problem (and any solutions) to 1 topic.  How can people learn from solutions and people's ideas, if they're spread over multiple topics, when they all relate to the same part???

[Anonymous]

I gotta take this step by step so I can learn it, if you don't mind. I have the orginal file here in an attachment. 

So what you did was

1) Remove the shady bit in the middle using delete face. 

2) You created a flat part between 2 sides. 

This is where you lost me. Did you just sketch something between the two sides, extruded it and then used offset surface = 0 mm? 

[Anonymous]

I get to the part where I have to stitch the two surfaces together and I get an error message. 

[sam_m]

so... what I've done and the reason, from your original file:



1) roll up the end of part, so we've got the original part with no commands/features active.

2) offset the inside face with zero distance to get a copy of these faces as a surface. I'm wanting to create the part as a surface, much like the final sheet metal drawing, with no need to worry about the side walls and creating features with a matching outer and inner face. So, use the "thicken/offset" command, change to surface output, change distance to 0, make sure it's set to face and not quilt and select the inside 5 faces.

3) now I want to remove the existing solid part, so I'm only left with above surface. I could do a new delete face command, but your original file has that, so I'll move the end of part below it, right click and edit feature, and select all faces (to speed this up I clicked the right button in the dialog saying "select lump or void" instead of the default "select individual faces" - select the part and click ok. Now I'm left with only the offset surface.

4) Now to remove the unwanted middle bit... I didn't know how much of the middle would be needed to be removed, and thought it might need more than the existing face, so I created a new work plane on the "good edge" and then offset one a nominal/guess distance away that looked ok. I used split face with this offset plane to cut the part and then delete face to remove the twisted face and this extra little bit.

5) to get it to unfold we need a flat section between the 2 outer faces. A loft between then would be twisted, but an extruded line should work. So, I used a new sketch on the "bent finger" bit and projected the two good edges. The new flat connecting face needs to cover the extremes, so I drew a line from the flat "good" edge next to the finger and the furthest away part of the angled edge. Extrude this as a surface "to" the furthest away point.

6) now we need to connect the angled face with the 2 holes to this new extrusion, so I used extend face and "to" the new face. So, now we need to remove the excess crap of the extrusion. We know we want to goto the end of this newly extended face, so I used split and this face to cut the extruded face. Now we need to sort out the sides, so I created a new sketch on the extruded face and projected the two ends of each side (the good edge at the end of the finger and the good edge at the end of the angled face with the 2 holes). Draw lines between them to be the outside edges of this face and use the split command to cut the extruded with the sketch (2 split commands, one for the left and right sides of the sketch). Use delete to remove the unwanted bits around the sides and top.

7) stitch the original offset surface and the new trimmed extrusion together, there should be no gaps. You now have a single surface representing the inside face of the sheet metal. But, we don't like sharp corners, so I used fillet to and a bend - the radius of this needs to be greater than the part's thickess, as one of these fillets is an "outside" - thinking about it, to be better, the outside fillet should be the value of the inside fillet + part thickness, to give the same bend radius for both bends.

😎 now thicken the part using "thicken/offset" and select "quilt" (to select all faces in 1 click), add 3 to the distance and make sure the direction is correct. sorted 😉

I hope that makes sense.

[Anonymous]

I get to this point. I removed the middle bit, I draw a line where there is a gap and I extruded the line. But then when I try to stitch it up I get an error message. Do you know what I'm doing wrong?

[sam_m · Accepted solution]

without wanting to sound rude, without a single word of thanks I wonder why I should keep going...  And saying it now is a little late...  You, know when you're driving and you can see someone wanting to pull out, so you slow down to let them out, most ppl wave to say thanks and you're like "that's cool, no problem" but when they just ignore you, doesn't it just frustrate?  People on here are just other Inventor users, we're not from Autodesk or paid to help (and are probably spending time during their working day to help, so it's potentially costing them cash), so a polite thanks here and there, marking posts as solutions, etc. will help in the future...

from your model:

1) you've offset the inside surfaces, fine.  But then you don't delete all the original part - you've selected all faces apart from the inside lot - so you've basically now got 2 sets of the same inside faces, 1 from the offset and the other from all the face deletes.  Use 1 approach or the other...  I used the offset 'cos it's easier for more complex models - you only need to select the inside faces and then delete the entire void, without having to click every other face.

2) the stitch is probably failing because the surfaces aren't connected properly.  You need to extend the face with the 2 holes and then cut down the new extruded face, so the ends of each face are all touching.  Look back at my model - I trimmed it all down before stitching it all together.

[Anonymous]

My apologies. You are of course right. It was very rude of me. You don't need to keep going. That's ok. I appreciate you folding it out for me and for learning me a new way to do this. 

I am very new to Inventor so any help I get from this community is much appreciated. Usually in my other posts I have been very thankful but I didn't see your reply until this morning when I got back to work and posted the other post. Again I hope you will accept my apology and I thank you for your help. 

[sam_m]

surfaces can take a while to get your head around, but when you do it helps a lot as it gives you another way to approach a problem.

In all honesty I would highly suggest going through JD Mather's great surface tutorials here:

http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm

they're a few years old now, so were setup with an older version of Inventor in mind, but they should still give you a better in sight into surfaces than feeling like you're banging your head against the wall with your part.

[Anonymous]

I just went to the trimming surfaces, which you did somewhere on my part. That was very helpful.

So you are not working with Inventor? Just a hobby designer?