SV: Sheetmetal Flatpattern view not Flat

yepp.....ran into this problem in the beginning and got a few unusable parts
from the laser cutting company. After that I always create a new view, wich
I am sure is right and then name it "flat pattern view", or use the "insert
flat pattern view" option in the drawing mode.
Krister

Bob Draper <> skrev i
diskussionsgruppsmeddelandet:
....

 

Thanks for the confirmation,

Any idea what causes this?
Could it be extruding the base flange in the wrong direction?

Now that I can't trust flat-pattern to be flat. it'll be a big hassle
to create a new view each time around with hundreds of dxf's to
produce.

Be nice if someone was able to make a macro which would;
upon selecting a face,
1. flatten the part,
2. create a derived config called Flat
3. and create a normal-to-that-surface view

Even better would be to then;
4. open a 1:1 template called Dxf
5. insert that view onto the drawing
6. save as dxf in same folder as part with parts name.

bobd

 

Hi Rocheey,

That's a good tip for creating sm-flat-pattern config.
Up to now I've been opening up a drawing template and selecting
flat-pattern from a named-view option to get the flat child.

But the problem I was trying to get across is that my dxfs are indeed
created from a derived "true" sm-flat-pattern view, yet are not
deciphered as flat in Optimation software.
When I open the part, select the derived sm flat pattern config, and
a front view, it appears flat . If I then select the true flat face
and then select normal to view, the part appears to moves slightly
towards me.
I.ll mess with the base flange sketch planes and drw-dxf template ,
maybe that'll help

PS Just noticed Amada has a solidworks add-in "Sheetworks", ap100
interface,
ever messed with it?

bobd





(rocheey) wrote in message

 

?? You are creating a drawing "Front" view of a flat pattern? ??

No, I'm just using the models front view to look at the derived
child flatpattern view, which was created from parent when insertng
into a drawing.
I thought that when I go to that child flatconfig and select a front
view which the original sketch was created in, it would be the same 2d
as the drawing flatview. But when I highlight the face of the
flatpattern and select normal-to-view it moves slightly.....almost as
if my world view is off a bit,
story of my life ,... this is giving me a headache.

Makes sense,you may have identified the problem it here

Wow,now thats powerful stuff! People like you and Guy Edkins and Dom
"Flipper" inspire me to endeaver to learn more than just using the
software!

So I assume the external boundary can't be broken up and must have
tabs added to it?

You know I ran into this very problem, tonight at work.
The CEO asked me to model(with solidworks) a golf divot/spike tool
from 14ga SS with our logo etched on it. He wanted 300 for important
CEO stuff. (its good to be king)
So I created two dxfs , 1 with complete internal logo and outer
boundary, the other just the external boundary.
I then generated 2 identical nests of 14 in a row, fron the 2 dxf's.
( our 2000 watt amada has a 125kb filesize limit)
Edited the GLA file in the first nest, replacing all the cutting
conditions to e10 etch, and had the laser operator run the etch nest
first, than overlay the cut nest after to produce the parts.
Well I had to add a couple tabs (microjoints) as they popped up over
the rollers and wasn't able to use the trap door, as usual.
Anyway the CEO rejected the parts because of the brown marring from
the initial cut. So I added a leadin cut, but with our Opti software
the leadin disappears when using tabs. Apparently we gave that option
up for under the clamp and common line cutting. Optimation is limited
in that regard. And our laser operators cant dial in the conditions on
thicker stainless to allow a pierce cut, 16ga max.
So I tried breaking up the boundary of the "cut" dxf into an open
contour that would create microjoints as you spoke of with internal
cutouts. Theoretically I would still have my leadin and tabs.
Rejected! The only solution left was to run the etch nest, then run
the cut nest with leadins but no tabs, forcing the operator to stop
the laser each time 1 part was cut thru.

Are you able to manipulate leadins, pierces and cutting conditions
with your app, or do you leave that to the laser operator? Or perhaps
your product doesn't require a variety of settings.?

seeya
bobd

 

I thought that when I go to that child flatconfig and select a front

Ahhh, sounds like your unfolding software is like API/Amada... wants
to grab and unfold directly from the model, and not from a 2d drawing.
Hell, Amada wont even unfold the part if it has the Flat pattern
FEATURE .. (it needs to have Insert bends/Process bends)

I got sick of the crap I was getting ( as well as sometimes losing the
orthagonal flat orientations). I dump the flat pattern to a drawing
doc, parse the geometry right from the drawing view, and write to
whatever file format is needed.

Again, Amada/API will just 'disappear' from the screen (crash) if
everything isnt right with the outside boundary. Thing is, in Amada
laser (but not Punch)you HAVE to break up the geometry into peices to
do any type of repositioning cuts, so you just have to hurry up and
write the NC code, and then NOT save your work. (Redo the same work
every time for every part!)

sigh,,, I'm still doing much the same.. Im suprised none of these CAM
apps has a
"Government Work" module that will let you take off the training
wheels
in instances like this. Im slowly working in my own NC Code generator,
at least for the Laser. I'll probably end up nesting and toolpathing
flat patterns directly from a SW drawing, possibly using blocks tied
to dxf files, if the flat patterns dog the app down too much.

I used to write 4-5 axis CAM apps (machining centers/Mill), and the
thought of these companies charging four figures, for a single tool,
and only 2 axes, and not being able to do it correctly, well, .....
err, dont get me going.

I gave up on trying to post clean code and now have my own "post" that
takes OUT the crap (like trying to put in a .100" leadin cut for a
..025 diameter hole) and puts IN the crap they missed (like changing
the Gas settings for engraving, etc, while the tool is positioning,
and NOT on the way down; or
removing the redundant cuts myself, because the common-line cutting is
so fragile: they apparently tied the common cutting to the GEOMETRY,
and not the TOOLPATH. If it senses any probs in the Geometry, the
Toolpath fails.

As far as microjoints go, I put in a bare minimum on the part (again,
Microjoints were tied to the damn geometry, and not the toolpath:
Microjoints are just places where you DONT CUT. Ive never recieved a
model from a customer that required a microjoint FEATURE)

I wrote a 9000-series NC-Control macro that hooks G01, and
automatically replace the G01 cuts with my own macro calls .. the NC
macro allows the operators to specify how wide, and how far apart it
should "add" a skip in the cuts. Comes in handy when the part starts
warping, ie, every 12 inches, add a .030 "microjoint", etc,etc.