Flat vs Model vs W/ trim on/off

Phenom
Phenom

I have a need to show a part in two different states within a single draft.

 

For the flat pattern, I need to turn some trims off

For showing how it's bent, I have to turn some trims on

 

Why: Because it's imposible to fold the part in the computer where as in reality the part can bend.

The solution was to add a few fictitional trims so I could get the model folded up. But now I have to figure out how to use both in a single draft.

 

Is there a way to do this without using two seporate models?

11 REPLIES

Re: Flat vs Model vs W/ trim on/off

PLM World Member Phenom PLM World Member Phenom
PLM World Member Phenom

Just off the top of my head could you use simplify and then pick whether to use the simplified part in some views and the designed part in others?

 

Kyle

Kyle Joiner
IPA LLC
ST9 MP1

Re: Flat vs Model vs W/ trim on/off

Phenom
Phenom

Hi,

 

I suggest using Multibody modelling to this:

 

 

FOP without populating should be a "big gun" in this case...

 

BR,

Imics
http://solidedgest.wordpress.com/

Re: Flat vs Model vs W/ trim on/off

Phenom
Phenom

Thank you Imics,

 

Thats very cool. I wish I could read your language.

 

I can't use FOP/FOA because I'm using plane control. Have not had time to move over to Sync to handle the overall dimensions. I would have to start all my models over because Sync can't see ordered features.

 

Very early one I found the using planes to control model size blows up FOP/FOA somehow. Can't remember exctly how.

 

I have posted the model this is about in another thread called "Difficult sheet metal corners"

Re: Flat vs Model vs W/ trim on/off

PLM World Member Legend PLM World Member Legend
PLM World Member Legend

How about using suppression variables?  That will likely do what you want to do.

 

Have a look at http://community.plm.automation.siemens.com/t5/Solid-Edge-Forum/Removing-Cutouts-from-a-Flattened-Pa...

 

 

 

Cheers,

 

Chris

Re: Flat vs Model vs W/ trim on/off

Phenom
Phenom

Thanks for all the Idea's.

 

The problem I'm having is that I need two different flat patterns.

 

One flat without the trims so I can dimension exactly the desired flat pattern

On flat with the trims, so that I can dimension all of the bend lines (the above flat does not have bend lines)

 

As a result, I think I'm stuck  with two files unless any of the other methods can be used to create a second flat from one file. If they can, how?

Re: Flat vs Model vs W/ trim on/off

PLM World Member Legend PLM World Member Legend
PLM World Member Legend

For this case don't use flat patterns.  Instead flatten it out using unbend features and create suppression variables for them as well.  By turning on and off the various features for each state that you wish to depict you will get what you want.  Then in the assembly file for the draft file you can bring in a separate instance of the part for each state that you wish to depict in the drawing.

Re: Flat vs Model vs W/ trim on/off

Phenom
Phenom

If I take that approach, then how  do I display both flat patterns?

 

If the part is not trimmed, it will not fold and not display the fold lines I need for back gage display.

If the part is trimmed, the flat pattern is not right.

 

I need both fold lines and a correct flat pattern.

 

If you are wondering about the specific details of the situation, take a look at a vid that Imics did for me in another thread "Difficult sheet metal corner"

 

I thought this thread would be a different tact on the problem.

Re: Flat vs Model vs W/ trim on/off

PLM World Member Legend PLM World Member Legend
PLM World Member Legend

To display both flat patterns on the drawing:

  1. In the part, create the suppression variables as appropriate, and make it an adjustable part.
  2. Create an assembly containing two instances of that part.  Bring the part in two times as adjustable so that you can turn on and off the appropriate suppresson variables for each instance of the part.  To do that you must create some assembly variables that will be used for controlling each instance of the part (i.e. the two "flat patterns").
  3. From there, create a draft file off that assembly file.  That takes care of the two flat patterns.  Please note that the flat pattern is not used at all here.  Instead, the views with the unbend features unsuppressed are used.

I don't have an answer for you regarding the fold lines.  Perhaps you can manually model them in as curves in the sheetmetal model.  Then get them to show up in the draft file by showing the appropriate curves.  Either that or use draw in view.

 

P.S.  Unfortunately Imics' video does not show for some reason.  I cannot even see the video link in that post!

Re: Flat vs Model vs W/ trim on/off

Phenom
Phenom

Thanks for the input.

 

Automatic generation of the bend line, start of bend,end of bend, are requirements. The model changes sizes frequently and I need my bend tables that are driven from those lines to update as a result.

 

In fact, I plan on pressing hard to request adding bend lines to the flat patterns in the model file. At some point I'm going to move all my bend table work to the model file from draft files.

 

My current work around is fairly simple.

1. I make a copy of the file, turn off the trims, then display that in the draft for the part that has the trims.

2 I link 3 dimensions (XYZ) between the two files to keep them in the same.

 

The only downside is if I need to edit, I now have to edit two files or recopy and link. Small price for the other things going on.

 

To make things worse, I have never used FOP/FOA, adjustable parts, or ever configured any switches to turn things on and off. There was one other feature you mentioned I have yet to use either. I don't have much time to learn complex procedures and I try to keep everything as simple as possible yet flexible enough to do what I need. I found that my plane control over models is a problem for FOP.FOA. I also found that the adjustable parts are not really adjustable the way I think of the term. They use adjustable to represent a fixed part stretching, not changing the part from 10" long to 30" long.