Sheetmetal bends and corner relief in 2005 SP3

Hi,

I've been looking at Solidworks 2004 as a possible replacement for Radan
for sheetmetal, it seems to have a few 'features' I'm unsure about ...

Take a base flange, 6mm sheet steel. add edge flanges and form a simple
open top box ... for added fun, make one of the sides with closed corners.

OK so far? .. with 'trim side bends' selected in the bend features you
can see it trim back the bends in sone of the corners to allow the metal
to be bent without nipping .. neat. the closed corners look right too.

if you *unfold* (note: thats unfold, not flat-pattern) the bends, you can
still see the correct shape for the closed corners, but the material
removed by 'trim side bends' seems to have been put back.

If you do a 'flat pattern' by unsuppressing the flat pattern feature, all
the corner relief seems to have gone awol. the raw outline is not the
same material shape that was used to prodcue the solid model .. all
trimmed bend corners relief has gone etc.

I'm now a bit confused between the differences of 'unfolding' all the
bends, and 'flat pattern'

So .. there seems to be a function to add some 'manual' corner relief,
choose a radius of circle, apply it in some random way to a few corners
... but then you cant *see* what it is that you are going to get when its
bent ...

Surely you should be able to see either the flat pattern of the metal
exactly as was used for the solidmodel, side bend trims and all, or you
should be able to bend up the flat pattern with its circular corner
reliefs added, but as it stands it seems to be a case of cutting it out,
bending it up on the press and having a look .. exactly waht I hoped 3d
solid modelling was getting away from, or am I missing something?

 

you're replacing apples with oranges, sw has no post-processor to generate
g-code ... unless of course your machines don't require g-code.

 

err ... thanks, but, if you read my post, I think you'll find I didn't
mention GCODE once ... my question relates entirely to how sw flattens a
folded sheetmetal part and why the flat pattern lacks the features of the
folded version ...

fwiw, gcode generation will be handled by exporting the flat pattern to a .dwg
file and nesting it with Turbonest, which generates gcode for the laser.

My question is purely related to why doesnt the sw flat pattern match the
folded version and how does 'unfold' al bends differ from 'flat pattern'
.... the gcode is easy once you get a flat pattern that matches your
folded part.

 

Hi Robin,

Perhaps you need to look into something like merry-mech to generate
your g-code for your machines. Solidworks is a CAD package, not a CAM
package, so when you go to program your laser and turret press, keep
in mind that SolidWorks will not be of much use unless you . . . .

(just kidding)

Yes, what you describe is a really nasty little bug and completely
flakey (I agree with you there). The trim notch does disappear once a
closed corner is added with an unfold. The problem even persists once
the unfold feature is gone.

While I would not stoop to defend such a silly bug, I would like to
say that one is able to attain much better results with alternate
methods.

The closed corner feature is a little anemic to start and the "trim
side bends" while being a convenience switch is (as you proved)
flakey. In my mind, the "hard truth" is that modeling "one's own"
clearances into the part, while it takes a little longer, makes for a
rock solid model that does not do the stuff you see here.

The reason unfold exists is to make cuts accross a bend (also a silly
and inefficient move most of the time), to make sequential configs
(very useful but also attainable through bend suppression without the
unfold feature). The flat pattern is a nice little state of the model
that can flatten all the panels and weld them into a single panel (no
line-line-line output when processing the flat in CAM - very nice
indeed) and also gives you a "corner treatment" if you want one.

Corner treatment is a manufacuring convenience only and the corner
treatment geometry cannot be propogated "backwards" into the "folded"
model. This is an extermely lame aspect of this feature as it creates
and even promotes a geometric disparity between the designed and
fabricated part. Another note on the corner treatments: Nearly any
cut or "fill in" can be effected in the flat and be propogated back
into the model if the "right" techniques are used.

Yeah, what you are missing is that the "convenience features" (side
trim, closed corners, edge flange, etc) are only conveniences during
design, not during fabrication and flattening (ie flakey & buggy). I
assure you that solidworks can do a smash up job unfolding sheet metal
when other more robust techniques are used. In particular,
self-designed clearences will not fall apart like this one. Closed
corners can be attained through alternate means. Using "insert-bends"
instead of "base flange" will not hinder ones modeling methods ->>
insert-bends allows some more modeling techniques that are not
avaialable when using "base flange" (ok i confess, I have yet to use a
base-flange on a production part - ok I did use it once but only
because I inherited the part).

One comment on Radan/SolidWorks - One area that you will see
solidworks outshine most other products is in its ability to make
sequential configurations of a part as it travels thru the
manufacturing process (flat-first form- second form - final state).
If you do any tooling that depends on a sequence of hits (progressive
or single hit series) you will find SolidWorks immensely valuable.
I'm not sure if radan will do sequential configs or incremental
unfolding. Also consider that if you are importing models into a
system (perhaps you are fabricating for many vendors), solidworks will
allow you to make a dumb model parametric with featureworks and in
many cases let you (incrementally) unfold imported models with no
additional work.

The really good news with solidworks is that once you learn to manage
and avoid the flakeyness, you will not have to deal with this type of
stuff. Under the hood it is quite capable of doing all your unfolding
accurately without losing geometry as your bug find points out.

Regards-

SMA

 

On Fri, 30 Jul 2004 05:12:08 +0100, Sean-Michael Adams wrote:

Hi Sean-Michael,

Thanks for the post, I read it and it seems to make sense. If you view
the 'trim side bends' etc as just convenience features that don;t come
out in the final flat pattern, then It sort of works I guess. I would
imagine that folding relatively thin (0.5 to 1.2mm) sheet, these
deficiencies can be ignored, but they do have to be addressed when
dealing with 6mm.

The essential point for me is that what I see on the solid model must be
what I see on the flat pattern and must be what I get out of the
machinery, or its all going to fail. I've already found the Bend-Tables
etc so I know we can match SW bending data to our tooling, and I;ve
written some macros to find all the sheet parts in an assembly, make
..drwg of the flat patttern and export them as .dwg files, so I know it
can be made to automate nicely with our CAM/nesting package ... its just the
flat-fattern generation from the solids that needs to be right ..

OK, That sounds interesting ... I have occasional use of a copy of SW
(ie, if I drive over to my friends place in an evening, when the staff
have gone home) so I can get to try these things ... I've certainly found
the modelling easier to deal with than Radan, and the user interface is a
lot nicer. Where Radan is better is in its treatment of corners ... when
you see a corner with trimmed side-bends, you unfold it and thats what
you get ... That bit of Radan is good. The rest of it is driving me up
the wall I imagine that shortly it will drive me to buying SW.

Is there a tutuorial or something that shows these 'right' techniques in
more detail? ... I did try unfolding the bends at one corner, applying a
circular 'extrude cut' and then refolding, but it complained that 'model
contains feature that cannot be folded' or something ... and as for
'insert bends' rather than 'base flange' .. I'm afraid that one has me
beat ... I thought the only way to start a sheet part was with
base-flange? no ...??

And what exactly do you mean by 'self designed clearances' ??

Anyway, thanks for the post, and you obviously do use this day to day for
sheetmetal, so it can be done ... I'm very interested to work out exactly
how ...

Now then .. about this gcode generation again )

Robin Szemeti.

 

err ... thanks, but, if you read my post, I think you'll find I didn't

err ... did you notice, i was just repying to your statement.

my impression of radan was that it's a cam system not cad. since radan has
the ability to nest & generate code, i just assumed that's what you were
using it for (in additon to modeling).

you can get exact results by bypassing sheetmetal tools and modeling as a
thin-extrude (sharp corners). apply sheetmetal feature after part is
completely modeled. then you will have folded and flattened parts that are
exact matches.

 

My question is purely related to why doesnt the sw flat pattern match the

In some respects/instances, Unfolding and flat patterns are the same.

The "Unfold" merely sets all the bends to 0 degrees. But it also
"rolls it back" to before certain features, if you look at the feature
manager.
Adding features in the design tree that come AFTER this spot in your
model
is the same as rolling back the feature manager to BEFORE you put
these features in.

Flat Patterns, as a feature, are normally the last feature in a config
and therefore other features will not dissapear when flattening in
this method.
A flat pattern FEATURE also optionally *processes* the edges,
simplifies and joins edges. This behaviour is on by default but can be
turned off.

Turning it off may give you a smidgen more accuracy, but you also find
you're
cutting a lot more smaller cuts (or nibbling if doing in a punch)

In addition, you can have a flat pattern CONFIGURATION, which is
created when you create a flat pattern view in a DRAWING. This is a
dervied/child configuration of the 3d model. Since it is derived, and
not the original 3d config, extra stuff can be done here that can be
specific to manufacturing operations that you may not want showing up
in the 'finished' #D part configuration.,

 

Hmm... Its not so much the 'smidgen more accuracy' its the fact that
essential features sometimes just disappear ... take the example I gave, a box with
a 'closed corner' ... the end piece overlaps the side flanges, and there
is a cutout in the corner to allow the piece to be bent. it shows quite
clearly in the 3d model ... and if you unfold that bend, you get a
diagonal line from the corner, out to the edge umm crap ascii art follows


--------------------
| |
| |
| |
\ /
|---- ----|
| |
| |

IE the left and right bits bend up, the top bit bends up to overlap the
left and right bits forming two closed corners ... the two diagoanl
cutaways allow the corners to be formed correctly

but .. as a flat pattern ..

--------------------
| |
| |
| |
| |
|---- ----|
| |
| |


ie the two diagonal cut-aways have gone, yielding an unbendable part ...
it is possible to add corner treatments it seems to the flat pattern,
(circular cut aways at the corners) but you can;t see what thats going to
look like in 3D ...

Sometimes the closed corner genrates that sort of corner (above)
sometimes it generates a 'T' shape ... flat pattern follows ...

--------------------
| |
| |
| |
-| |-
|----| |----|
| |
| |

quite whay its ometime ones way, sometimes another, sometimes visible in
the flat pattern, sometime not is not celar to me. I've tried
checking/uncheckig the various 'corner treatment' and 'simply' options in
flat pattern, to no great effect.


<time passes>

Ahhh ... OK, I seem to have a bit more insight now ..

If, you end up with that funny diagonal thing, then its worng ... that
seems to be a bug somewhere in the folding and add closed corners.

The problem is related to the fact you can't add a closed corner to a
'material outside' bend feature, but need to use a 'bend outside' feature
and then apply an negative 'offset' to the bend to bring the face the
flange back almost flush with the sides

If you use a 'bend outside' and a negative offset, then the closed corner
feature seems to work correctly.

If you use a material outisde and a positive offset, then it does not ...

I can sort of see why it fails to add a closed corner to a /material
outside/ feature, in that it extends the face of the feature until it
meets the side and then stops, thats fair enough. It seems to go wrong
when you offset the bend 0.5mm to allow the closed corner to extend to
the edge. It does extend to the edge, but you get a weird diagonal
corner.

The solution I suspect is simply for someone to fix SW 'closed corner'
feature so it can extend the face of a 'material outside' feature
correctly.

Anyway, now I have figured out the workaround, its not a problem ...

toodle pip!

 

On Fri, 30 Jul 2004 16:40:02 +0100, Robin Szemeti wrote:

to follow up my own posting .. again

It seems the workaround of making the edge flange 'bend outside' and then
offsetting it -ve by the bend radius - 0.1mm (in effect placing the
inside face of the edge flange 0.1mm above the side flanges) does work
nicely, producing nicely trimmed side bends, and allowing you to add a
'closed corner' to extend the edge flange to overlap the side flanges.

It works right until you set the bend radius >= 0.5 * material thickness,
then it all falls apart again

Since the standard bend radius we use is bend radius = material thickness
(we bend with tool V = 6 * material thickness as a minimum, and expect to
get bend radii of tool V / 6. On heavy jobs tool V = thickness * 8 or
more is used )

Anyway, it seems I cant get it to work with our normal bend radii .. I
guess I can fool the bend corrections by putting the bend allowance for a
4mm radii in the 1mm radii column, but it seems a bit of a fudge ...

any other clues gratefully received ...

 

Try unchecking the simplify bend box in flat pattern properties