Sheet metal twist??

Is it possible using sheet metal commands (or others) to twist an object,
equivalent to holding a plastic ruler by its ends and twisting one end
through 90deg?

I can get an approximation of this effect using a loft, but it's not
visually perfect, and it can't be unfolded.

I've also had a go with the "deform" tool, but I couldn't get that to work.

I'm on SW2004sp5.
Has this capability been added since?

TIA
John Harland

 

SW2005 has the flex feature that will allow the type of twist that you
are looking for.

 

But it wont flat pattern the flex feature.

 

Have you tried a lofted bend?

 

Can you unfold anything, that is not linear bends ? This deformation
will stretch the material on the edges and is therefore not linear.

Leo

 

In this case, aren't you starting with the flat?

 

I've got some examples of lofted bends that do some twists on my
website:

http://mysite.verizon.net/~mjlombard/

Go to the SW Parts link.

matt

 

John H skrev:

If you simply like to have it like the ruler you mentioned, do like
this:
1) Select a plane and sketch a line with the midpoint in origin. The
length should be as the width of the "ruler". Close the sketch.
2) Create another plane in a distance (Ruler length) from the first
plane and sketch a line on this, 90deg to the first line.
3) Select Insert/Sheet Metal/Lofted bends. Select the two sketches and
enter the material thickness.
There you have your twisted "ruler" and it is possible to flatten.

 

Thanks for the suggestion. I hadn't noticed "lofted bend" under the sheet
metal menu, and for a minute I thought it was going to be the ideal
solution.

I can create a "twisted ruler" with the command, but what if I want to (say)
grip the ruler 1/3 the way in from each end and twist the middle 1/3 only,
leaving the ends flat (or with other tabs etc)?

It seems like lofted bends only work if they are the first and only sheet
metal feature in the part.
Is this the case?

 

I am not sure but could you pull a 8888 0 degree edge flange bend off
the end?

Ben

I am not at my computer to test this so I am not sure if this is
possible, probably not as the end would be scalloped in the unfoled
state therefore not a flat edge to pull the flange....

 

I am not sure but could you pull a 0 degree edge flange bend off the end?

Ben

I am not at my computer to test this so I am not sure if this is
possible, probably not as the end would be scalloped in the unfolded
state therefore not a flat edge to pull the flange....

 

Ben,
I don't seem able to do any sheet metal commands on it.

John

 

Unfortunately there seems to be some limitations. I. e. it is not
possible to use more than two profiles for the lofted bends.
This will probably create some stretching and deforming and SolidWorks
couldn't handle this.
For this type of sheet metal features I believe a software like
FastBlank is required. This is possible to integrate with SolidWorks as
a plug in.

 

Curious..

Here, try this (it is not a solution to the problem but interesting none
the less.

Sample models of what I have discussed here are at
http://members.shaw.ca/b.eadie/Twist.zip

Make two parts part one will have a line sketch on the front plane, next
make a plane some arbitrary distance from the front plane and parallel.
sketch another line (both lines are mated at the midpoint to the origin)
the same length at 90 degrees and loft a sheet metal part on this and
flatten it. The resulting flat pattern has arcs at the ends.

Next make another part and draw a circle with a diameter to match the
length on the line in part one on the front plane and create a 90 degree
helix at the same distance the planes are separated in part one. do this
again and crate another helix but at 180 degrees out from the other at
the same rotation (counter clockwise if that is what you used). Next
create 2 3d sketches based on one of the helixs'. and another for the
other helix (sheet metal will not loft off of a helix) and then loft a
sheet metal part off the 2 3d sketches and look at the flat pattern. it
is perfectly square....

I wonder if on some of my lofted bends in the past could have been much
simpler if I had used a different modeling technique? This non
conformity for the flat pattern is most likely the reason we cant add
anything to a lofted sheet metal part as given it is the same part but
two possible flat patterns then there is some problems with the lofting
algorithm.

Ben

..

 

Hi Ben,

I can't open your parts because I'm on SW2004.

John

 

Sorry I don't have 2004 so I cannot help you the text can walk you
through building the models though

Ben

 

I have been trying for days to do the same thing. Have you found a way
yet. I have been trying to use the louver idea in Sheet Metal |
Forming Tool. While it will not give me a flattened sheet metal part
it could get me to what I want as a finished product. But no luck yet.
David C.

 

I have been trying for days to do the same thing. Have you found a way
yet. I have been trying to use the louver idea in Sheet Metal |
Forming Tool. While it will not give me a flattened sheet metal part
it could get me to what I want as a finished product. But no luck yet.
David C.