SolidWorks won't let me unfold the sheet petal part I have pictured in pic 1. Pic 2 is as far as it will let me go. Can someone please tell me what I'm doing wrong?
First insert a Sketch in the front plane
Add a plane
Select the New Plane and the Sketch and Insert/Derived Sketch
I did forget to radius the corners, a must when making a sheet metal loft part
Select both sketches and the lofted-bend feature
Adjust your thickness etc.... You can adjust your length by increasing or decreasing the plane1 dimension
Final Part ---
At the nose of the part you used a spline or a conical curve, can you change the sketch by using circles/radius lines instead, that should do the trick
Is there a way to do this and still get the same shape that I have in the first picture?
The sketch is under defined and can move, first thing I would do is to fully define your sketch by applying dimensions to what you have. then take the conical sketch and add points and lock them in with dimensions then draw circles or radius's and trim as required. There is one thing I just though of when I was typing, does your version allow you to do lofted bends?
If so then add a plane the distance of the length of your part and make a derived sketch on to that plane and do a sheet metal loft, that may work...
Works with lofted bends - didn't change anything except the fillets
The only thing I needed to do was add fillets in the sharp corners
Would you mind attaching the sldprt file? Not sure how to do lofted bends.
Do you have 2015 ?
I have SW 2013.
Thank you very much for this. The shape is not quite what I am trying to get. Attached is an example of the shape I would like the make. The distance horizontally is 2mm longer than the distance vertically. Would this shape be possible?
Maybe sheet metal is not the way to go? I only chose it because it allows me to flatten, which makes it very easy to insert a fill pattern into the walls of this model.
It also allows me to add rings orbiting the model using a linear pattern.
Should work fine -
Followed the steps but got stuck at running a loft bend. SolidWorks is not allowing me to choose my 2 sketches.
The sketch is:
After selecting the two sketches and clicking Lofted-Bend, the error I get is:
And when I click OK, I cannot add the sketches to the Profiles section.
What am I doing wrong? I used a spline to sketch the curved part of my object. Is that correct?
Thanks for your help!
You need a gap in both sketches
Thank you, I figured you make the trim after. I ran into a problem right at the end where I am trying to fold it back up after applying a fill pattern and then a linear pattern of a ring. Below is what I did.
Now when I do the fold it gives me an error:
I have tried numerous ways to fix this but it has not worked. Edge 1 was the only one it lets me select and I have tried with every combination of bends.
If you can please tell me what I am doing wrong, I would sincerely appreciate it!
Could you upload the part? Or make a straight cut where the error shows up
Attached is the part. I'm not sure what you meant by straight cut where the error shows up.
The error shows up when I select this edge and click collect all bends:
The profiles will give you an issue with the bending, what I meant by the cut - it mentions in your screen shot that there is a beveled edge, I thought it might help if you add another cut and then reselect the edge. The part you uploaded doesn't have those features it is the same as the original one you uploaded
I attached the wrong file, so sorry about that. Attached is the correct one. Will try your suggestion as well.
SolidWorks Sheet metal has no idea what to do with the extrudes and cuts in the re-bending process - For future reference you can also select a face rather than and edge for your bending...
Now you can get the flat layout which will give you a true length, however to show everything in a drawing you would need to model it, which can be a challenge.
I was able to fold it back up after removing the extruded rings.
Now I am trying to extrude a new set of rings around it but I am having trouble selecting an axis of rotation. Below is the sketch I am trying to revolve around my model.
For the axis of rotation, I tried using a vertical line going up and through the middle of cylinder and it would not let me select it. Then I tried using the sketch seen in this picture (in blue). This is a new sketch I made on top of the cylinder (not an existing one that was used to make the cylinder using Sheet Metal earlier). It's not letting me select this either. I did this once with the cylinder being a true cylinder (extrusion of a perfect circle) and I was able to revolve a ring around it easily. Not sure what I am doing wrong. If you can take a look I would greatly appreciate it! I have attached the file as well.
Mike I just noticed your last reply - What I would do is add a Sweep Feature, by using the outer edge as your path and then you will need to close up Sketch24 - a sweep profile needs to be closed geometry
Thank you very much John! Worked perfectly!
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