Your right. It’s easier to change the sketch to over
form too. Using a radius length dim to lock the length, then change
the angle… the radius is automatic. Very kool.
"I suppose I could have changed the sketch and made 2
configs… but that scared me."
I would still go about using the assembly, but I would use
solidworks explorer and save the master file into a different name.
So then you can still use the original sketch and you can change
the dims, angles, radius, etc with the piece of mind knowing that
you are not messing with the master file. After the copy and rename
you can then put them into the assembly file so you have the master
to compare to while you are changing the geometryof the copied
part.
This to me seems like a more streamlined approach rather than
having to imake a flat and then inserting a bunch of sketched
bends.
Thought I’d sent a follow up. I needed to check my flat
anyway, since I laboriously did it in 2d… so I decided to
model the part with my new found knowledge.
I can’t show the part of course, the here’s the
tree. I’m using both miter bends and flat suppression. As
well as modeling crushed features under the flat feature to show
areas that can’t be unfolded.
You see the master sketch at the top. That defines the form
profiles and splits. The miter sketches are converted from the
master. I have 2 forms where a 5 deg change significantly effects
the tool. By changing the master I could optimize the angle
effortlessly.
Boy do I love grouping feature in folders, makes the tree so
clean and the entire group can be suppressed. You see the
“flat features” folder… the first feature in
there unfolds the whole part, then all kinds of cuts and fillets
are added to the part that would have been impossible in the formed
position. Last feature re-forms the part. What a mess the tree
would be without folders.
There are 8 configs showing the part in different stages of
being formed. The only features I’m un/suppressing occur
below the flatten. I’m really shocked by how well thought out
SWx is. The ability to model features below the flat and isolate
them within different configs allows the impossible to be
modeled… in a single file.
I had to model features on existing forms… below the
flat feature… that were outside of suppressed flatten forms.
(maybe “yet to be bent” forms describes it better) Then
when the flatten forms were unsuppressed… the modeled
features moved with the whole leg. It’s hard to describe, but
I was floored when it worked. Look at the bottom of the expanded
flatten feature, there’s a folder named Sketch
Transformations. Whats that? I’m guessing that’s the
matrix for the features below the flat feature (in the
“finger CRUSHED” folder) that moved when the flatten
bends were suppressed.
I did have to create separate files to make the
“overformed” profiles. I was hoping a flattened bend
could be reformed with a different bend radius and angle, but no.
Overforming for springback compensation is really a special case.
I’m not expecting miracles.
Well, as you can tell, I’m real happy. I suppose
youngin’s just expect software to do what they want, but
I’ve done probably 400-600 flats manually in 2d. I know the
math behind whats going on and all the special circumstances that
have to be dealt with… and I’m blown a way.
Have you thought of inserting the file into an assembly and
then making your own part around that one. Then you could change
the bend radius and angles to your liking (overforming) and it
would still match the original file. That might be more work than
needed, but just a thought.
I see. The jog offers limited uses though. The flange feature
sort of works, but it’s not tang. A small flat usually
won’t be a problem but it’s tedious to add since you
either have to do math or punch in numbers trial and error to get a
real small and consistant flat.
Apparently, it’s hard to run bends tangent. Inventor is
the same way, required a flat. I wonder if that is real hard to do,
or just requires a whole lot of programming for a few special
cases.
Jeeze, I guess I didn’t. Thank You. This SW is great.
Maybe another big problem I’m having is also easy. Lets
say I need to form this big radius in 3 hits. Basically splitting
the form into 3 separate forms. What’s the best way to do
this?
I was hoping a “split entities” feature on the
radius would split the form into 2. but no.
Diemaker,
I've attached a PDF showing two different ways to achieve
tangent bends. The one on the left is done using the flange feature
with something less that 90° angles and minimal distance. The
one on the right is the jog feature. This one has various
parameters that you can set, including "Fix projected length" so
that your flat pattern doesn't change in length...
Jeff Mirisola, CSWP
CAD Administrator
HySecurity Gate Operators
SW2007 SP0
XP Pro, Dell M90, Intel 2 Duo Core, 2GHz, 2 GB RAM, Nvidia
Quadro 2500M
THANKS. I never noticed that, SW is full of little Easter
eggs.
Here’s the part I’m making. Progressively bent
with a few overformed stations to make it complicated. So, I really
can’t use the individual bend suppression for the finished
part… this time. But it would have helped at the beginning
when I was experimenting with different bend sequences.
I made this progressively bent part by creating the whole
profile as a base, flatten, put the part in an assy. Add new part
to assy. Convert the bend lines from flat to new part. then used
sketched bend to add the bends back in.
I think sketched bends are the only way to break forms up and
change angles and such without changing the overall length of the
flat. But, I still want to create tangent bends one feature at a
time…. I thought, maybe the HEM feature can do that.
And it can, HEM has a curl option that allows just a
“bend”. But I can’t add anything to the end of
the hem. I accept there must be a little flat between bends.
I’ve made flats only .0005” wide with success. But I
can’t add anything to the end of the HEM. It will model, but
disappears when flattened. The attached model shows a hem with an
extrusion on the end, if this had worked, I would have made the
extrusion .0005” long and modeled another HEM … to get
a “S” shape.
So you might think I’m just creating a flange with a
.0005” straight… I am. But there is no option in FLANGE
to control straight above the radius. The 2 length options measure
from sharp corner, inside or outside. So getting an exact straight
above bend requires extra calculations.
I’m sure most don’t have to deal with all this
crap. They only design the part. I design the tools to make the
part. This part also has 3 big ribs, dimples, holes, offset form,
fingers with crushed formed details, has to make 2.7 million parts
at 35 per minute and hold accuracy of +/-.010.
I took your sample part and added 3 configurations to it to
demonstrate 1, 2, or 3 bends.
This trick is to suppress the appropriate
Flatten-<BaseBendx> feature in the Flat-Pattern1 entry in the
Feature Manager.
The Flatten-all tool is just a convenience - it simply
UNsupresses all of the flattening features to make a flat pattern.
With the flatten features suppressed, the part appears to be bent.
Gerald Davis CSWP
SW07 SP1.1 Office Professional
2GB / Opteron 175 / FX3400 / ASUS A8N32-SLI
http://www.cosug.com Colorado
SolidWorks User Group
don't see how flatten unfolds individual bends. help for
Flatten says:
"To flatten one or more individual bends, add an Unfold
feature"
heres a simple example.part. flatten the middle bend (50
degree bend)
the only way i know to model this part is to sketch the
profile and make a base feature from the sketck. so un-bend does
not work because there is no bend feature. I know no way to create
a bend thats only 50 deg.
Is there a way to create sheet metal with tangent form radii
where each form can be un-bent individually?
The jpg shows a part with tang radii. It was made with one
sketch and the BASE feature. But it only goes from formed to flat.
I need to unbend each form. I don’t se any way to create this
one bend at a time… except by starting with the flat and
doing sketched bends leaving a small flat between each bend.
“Another thought... Take there model and save it as
something else, and then change the "br" and angles to what you
like.”
If I read you right, that exactly what I did. Since the
majority of the part was made from miter flanges, I saw no way to
change the radius and angles without changing the sketch. I suppose
I could have changed the sketch and made 2 configs… but that
scared me. So I made assy with the flat and converted the profile
and bend lines to new part. Then used sketch bends.
One option I wish SW had… When doing a sketched
bend… you need radius and angel…I’m sure SWx
could calculate the other given one and length of available
material to form. For example, sketch a line 1” away from
edge of material. Enter a radius and hit the “new
option”…DISTANCE. Then SWx would calculate the angle
based on how much material is there it could bend. Right now, if
you go .001 degrees over, bend fails.
In my case, doing the overforms, I wanted to sketch bend all
of the material between the sketch line and an existing form
knowing only an angle.
Outstanding, that’s exactly what I need. Triple Thx to
Aaron.
True tangent bends.
Ability to split a bend into multiple bends controlled by a
sketch.
Individual form control.
I wish I asked this 2 weeks ago. I could have easily
experimented with different form progressions. Because of the
complexity of this part it’s hard to draw the progression. I
solved most of the scenarios in my head then drew the one I choose.
But I got called on the carpet to prove why my choice was better
than the obvious choice. That’s what prompted me to ask about
tangent bends. I did search this group first but found nothing.
With miter flange I can draw a new scenario in ½ hour.
I got to gripe a little tho… MITER flange? I read about
that when I first got SW, but I never connected how to use it as a
“contour” flange. Look at the icon, read MITER…
every indication is that it’s a miter end treatment.
Well, I won’t forget about Miter flange now. This is a
big one for me. Thanks to every one.
I would still go about using the assembly, but I would use solidworks explorer and save the master file into a different name. So then you can still use the original sketch and you can change the dims, angles, radius, etc with the piece of mind knowing that you are not messing with the master file. After the copy and rename you can then put them into the assembly file so you have the master to compare to while you are changing the geometryof the copied part.
This to me seems like a more streamlined approach rather than having to imake a flat and then inserting a bunch of sketched bends.