Does anyone know if its possible to create a flat pattern of a sheet-metal mirror part.
I have Left and Right components in a sheet-metal assy when creating the drawings i would like to have a flat pattern for left and right components.
If you do the mirror component in assembly then it'll not be directly possible to get the flat pattern. Rather create a mirror configuration at part level and use that in assembly.
Could you tell me how to create mirror config at part level.
I have tryed insert mirror part at part level i still get the same thing a mirror part that i cant get a flat pattern.
Iam using solidworks 2009 sp0
Not sure if this will in SW09 but insert a body mirror as the last feature (make sure you don't merge the two bodies). Now create two config and delete one body in one and suppress mirror feature in another.
I am using SW2011 SP3.
I just did something similar. Create the mirrored part. Then use the Insert Bends feature to turn it back into sheetmetal. Your feature tree will look something like below and the part should flatten - as long as the original flattened.
I do this on a daily basis (SW 2011 SP3). It is not necessary to create a mirror part configuration. The steps are below and some of the steps have already been mentioned. I have found that these steps have to be done in order to get a complete flat pattern (i.e. bend lines, bend notes, etc.)
Step 1. Create your mirrored part.
Step 2. Use the insert bends command with your base flange being the same as the part you mirrored from and all of the settings (i.e. bend radius, k-factor etc...) matching your original part.
Step 3. Go to the configurations tab. Right click and create new configuration. Call this configuration Flat Pattern.
Step 4. While that configuration is active, click the flatten button.
Step 5. Create your drawing and drag your flat pattern into the page. You will notice that it is either not flat, or it is flat but is missing bend lines/notes.
Step 6. Once you have dragged and dropped the flat view onto the page, hit the green check mark.
Step 7. Click the view on the drawing and the menu will show up on the left of the screen. Click the drop down box under "Reference Configuration". Select the configuration that you created.
This is now an accurate flat pattern of the mirrored part with bend lines and notes just like a normal flat pattern. You might have to rotate/flip the view to get it to match your bent views but that is quite simple. This is how I do it daily.
Hope this helps.
I just tried the workflow (thru step 2) in your post of 6/6/11, and no joy. There's something about Process-Bends1 in the Feature Manager--SWx 2011 says the geometry in the bend region is too complex. It's a fairly simple part.
You can download a zipfile containing both the original and the mirrored parts here:
Thank for your help.
Try it again Andrew and follow all the steps to the letter. I downloaded your part and went through the sequence and it worked just fine for me.
That did the trick, thanks. I think I missed the part about breaking the link to the original part the first time I did it. But this raises the question--if I revise the original part in the future, does that mean I have to generate the mirrored part all over again?
I realize that the two flat patterns will be basically identical, but I think there's something to be said for the bend directions being associative. I could have a flat pattern view of the original part on the dwg of the mirrored part and manually overridden the bend directions, but I don't think that's a very elegant approach.
Thanks Mr Hampton, I needed the same answer ... the time you take to help one person helps many even months later.
I figure that most of the benefit of a mirrored sheet metal part is that both pieces can be made from the same flat layout. If the material has an outside face, then this benefit goes away, and I would be less eager top use the feature.
The burr or punch side is not an issue as long as it is called out on your drawing or part file. We have software that imports the files, we can flip them over using a similar mirror command. This assures you that both parts are the same. And maybe keeps them from charging you twice for programming if they charge for it!
The quickest and easiest way to do this (at least in SW 2014):
1. Create your initial part.
2. "Save As Copy" to make your new part file
3. Mirror the body.
4. Delete the original body.
That's it. This will allow you to make a proper Flat Pattern in your drawing.
(I just had this same question and was rather confused by the above replies, so I wrote my reseller's technical support and they gave me this wonderfully simple solution to the problem!)
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