CAN flat pattern part, but CANT in drawing? 2

[DerrickM]

ok, im stumped. i can flat pattern a sheet metal part in the part, but as soon as i try to in the drawing, it wont do it. when i do get it to work, it flat patterns ALL the views. im thinking the configuration got messed up somehow. ill post the part, if anyone can figure it out, it would be a HUGE help! i need these drawings done ASAP and i cant draw them... only other idea i have is to copy the part and let the copy be flat (so i dont mess up the assembly) and leave the original bent.

 

[ShaggyPE]

I didn't look at your file. Chances are I can't open it. I am using '06 here at work.

Don't know if these apply, but this may help
1. You can only do a flat pattern of a part, not an assembly.
2. When you insert a flat pattern into the drawing, it will create a configuration in the part called "flat pattern". within this config, it will simply unsuppress the flatten feature in the part. If your part already has a flat pattern config, then make sure that config has the flatten feature unsuppressed.
3. You need separate configs, one flat and one folded in order to display properly in the drawing. It sounds like you simply inserted a bunch of views and then unsuppressed the flatten feature in that one config and then all your views showed flat.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[CorBlimeyLimey]

Go to the Configuration Manager tab
Expand the config to show the derived flat-pattern config
Activate the flat-pattern config
Go back to the Feature Manager
Unsuppress the Flat-Pattern feature
Save the part

 

[Gurjjeet]

Okay, I know what you mean, I had same problem.
In my case (hopefully yours is the same)

I have a part which has sheetmetal boody & it flattens & everything is right. But when I try to insert the flat pattern view into an existing drawing which already have some views from other parts, it does not show any flat pattern view in view pallete.

This can be solved by creating a drawing from that particular sheetmetal part & then copy/cut & paste this into the existing file.

It seems that Solidworks only creates the Flat pattern configuration when inserting into a new file or the drawing file with views from same part only.

Hope it Helps

 

[CorBlimeyLimey]

Gurjjeet,

The views of any currently open SM part can be accessed from the drop-down list at the top of the View Pallette. There should be no need to cut and paste from another drawing.

 

[chavelo]

delete the derived configuration, then it will allow you to create the flat pattern

 

[Gupta65]

Go to configuration manager and switch to "DefaultSM-FLAT-PATTERN". Now come back to feature manager and unsupress "Flat-Pattern1" feature. Save you part and now check the drawing.

Deepak Gupta
SW2009 SP3.0
SW2007 SP5.0
MathCAD 14.0

 

[DerrickM]

ok, tried what corblimeylimey said, worked perfect! thanks for the help!

pulsating combustion rules!

 

[bvanhiel]

DerrickM,

This question is kind of tangent to what you were wanting to do, and it sounds like you've gotten the answers you needed, but I'll ask it anyways: Do you really need a flat pattern?

Most sheet metal vendors I work with ignore the SW generated flat pattern because they use their own internal bend tables that are specific to their equipment. They want all the part dimensions to be on the as-bent part.

I usually put the pattern on the drawing as an undimesioned view for reference, but I wouldn't let the lack of that view prevent me from releasing a part drawing.

-b