i had a difficulties with create a outer ring in sheetmetal so i created the whole in Feature cause it couldnt created in sheetmetal,now how can i get a flatten from this.also i couldnt convert it to the sheetmetal part.
and it is important for me to create it in a single part
i don't work with sheet metal, but i guess if you couldn't do it on sheet metal operations that means u can't flatten.
I think if u put some reliefe breaks/tears in that bottom flange that should work.
i tried different ways but i couldnt succeed
Hi Mohammad Ayoubiamirabad
Did you try?
thanks omur for you help and i appreciate it, during your way i got some error about k-factor.did you crash it too?
how can this flat pattern be right? The blue edge is much short than the red edge....this sheetmetal needs a lot of stretch to make up for that discepancy...a rectangular plate flat pattern seems awfully simplified
im agree.but this geometry is exagerated of what i meant.
in real my washer is small.
What k-factor you are using?
Why not Attach the actual *.sldprt file here?
Will you manufacture this part "in house" or will it be manufactured by an outside vendor?
In any case - significant stretching is going to occur in area beyond the bend zone - so I would expect a warning.
This is really more of a forming process than a strict bend.
You made me remember of an old part I did. It doesn't work with sheet metal either. I think we are not understanding the function of the part from the question. It seems odd that the print screen represent faithfully the real geometry, it does not seems possible to produce...
1-8EO786D wrote: It doesn't work with sheet metal either....it does not seems possible to produce...
It doesn't work with sheet metal either.
...it does not seems possible to produce...
Your part will work with sheet metal if it has a rip.
The OP's part is a deformation. (The finished shape is slightly different with the edges at the stretched rip.)
I mean it doesn't work in this sense:
That is a very different problem.
Mohammad Ayoubiamirabad wrote: thanks omur for you help and i appreciate it, during your way i got some error about k-factor.did you crash it too?
Mohammad Ayoubiamirabad wrote:
Use bendobend allowance, not k factors.
Elmar Klammer wrote: how can this flat pattern be right? The blue edge is much short than the red edge....this sheetmetal needs a lot of stretch to make up for that discepancy...a rectangular plate flat pattern seems awfully simplified
Elmar Klammer wrote:
I did not test its accuracy, I just drew it.
Ask yourself, how much sense does it make to draw something that can't be made. It is important to understand that some of the sheetmetal features are simple automated modeling routines. They merely get you a 3D model, but the information provided in the flat layout is in most cases unusable. The swept flange, the way you drew is falls into this category. The ratio between flange length, bend angle and roll diameter will limit the use of such a feature. I see it all too often that operators draw up models that lack technical know-how. I would put money down that no 0.1% of all users that have used the lofted sheetmetal feature have actually understood the limitations it comes with or read the info in the help file. I see it over and over again, where models are built using the wrong features. And in most cases operators have little knowledge of what they actually do. Automated scripting buttons are a poor replacement for actual transferable knowledge and skill set.
As has been stated in this thread already you can't make this part in SW sheet metal because you can't reasonably fold this part from sheet metal. SW sheet metal is a function for sheet metal folding not sheet metal forming.
Think about what is happening in the material when you're attempting to form the flange. As you move further and further from the from the bend line the material has to stretch. If you attempted to do this you would end up with random tears in your flange, more or less depending on length of the flange, material type etc etc.
A decent rule of thumb for SW sheet metal is that if the bend line isn't straight and going across a straight surface...it's not meant to be done in SW sheet metal.
Sheet metal mostly for bend, rolled parts.
It could work for mild form, punch, press part.
The part you show cannot be bend.
Bend and roll, maybe.
i saw they bend like this with turning machine in companies
It call spinning.
Still not bending. The metal stretch a lot. Result parts are thinner.
I work in spinning before.
You cannot spun with the cut. Need to cut it after.
Fast Extreme Big Metal Spinning Process Working, Amazing CNC Metal Spinning Machine - YouTube
yeah it became thinner,
so with no way to do it in sheetmetal,how can i get an engineering drawing for it?
Mohammad Ayoubiamirabad wrote: i saw they bend like this with turning machine in companies
Like Fredrick said, that's spinning.
There are all sorts of ways to manipulate metal and all sorts of ways to model things in SW. The Sheet metal function in SW is meant for bending sheet metal not forming. Even if you use the form tool in SW sheetmetal it, at least to my knowledge, will not create a flat pattern.
Forms like this are done all the time in dies, spinning, forming etc etc. SW sheetmetal is not meant for this. However there are lots and lots of die/Mold programs that will do this.
Mohammad Ayoubiamirabad wrote: yeah it became thinner,so with no way to do it in sheetmetal,how can i get an engineering drawing for it?
Draw it the way you want it using revolve. Call out the material you want used and the specs on the thinning that is acceptable and let the person who has to make it do the rest.
If they spin it they will approach it differently than if they deep draw it. Do you even need it to be a single piece. You could do this in sheet metal as a weldment. Roll the top weld on the the flange.
so due to your reply,
how can we a get an engineering drawing to manufacuring?
cause we cant use solidworks sheetmetal
Mohammad Ayoubiamirabad wrote: so due to your reply,how can we a get an engineering drawing to manufacuring?cause we cant use solidworks sheetmetal
Not sure I understand the problem. As I said draw it the way you want it and put the specifications on it and send it to manufacturing.
Manufacturing might make it from sheet metal by using a weldment, roll it, deep draw it or turn it from a solid. As long as it meets the specs on the drawing it's a good part.
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