Contour Flanges

[Anonymous]

I am building an exterior for a product housing out of sheet metal, and we need a left hand and right hand due to the manufacturing capabilities of our plant. I have created both as countour flanges and the sketches mirror each other off of a .040 centerline for .008 tolerance between the 2 parts that are 20 GA (.036), however when they are created the LH is longer. Im sure this has something to do with the radius or something, but i cannot figure it out. Parameters on the "Countour Flange" Option are both the same so any help would be greatly appreciated. I did this eact same thing in a smaller (dimensionally) drawing and had no problems at all.

[CCarreiras]

Hi!

Basic.... one contour flange is growing thickness outside the sketch.... the other is thicken inside the sketch....

Tip: To create mirror parts, you can create then using the tool "Mirror" in assembly context.

Also read about creating mirror parts with "derive part". You are repeating work.

[Anonymous]

Carlos,

I understand the parts are doing that, but if you look inside the Contour Flange Options both are set to push thickness to the inside, so why is one different than the other?

Also, the "Mirror Part" command creates a non-editable solid. When we get to production we need to be able to make a flat pattern out of the metal so that it can be manufactured. For prototype drawings I did use the mirror part command, but that command will not work now that we are past prototype stages. Any clue as to why one is making the metal go outside instead of inside?

[CCarreiras]

Of course you can Flat pattern the derive part. Just edit the Thickness in the rule.

When you convert the derive to sheet metal, also you have to edit the thickness in the rule, because it comes with the template thickness.

Edit the thickness, it will flat.

[johnsonshiue · Accepted solution]

Hi! Inside and outside may depend on how the sketch was created. If you set the direction of one part the other way, are you seeing consistent behavior on both now? If not, maybe the two sketches are not the same. Please post the file here or send it to me directly (johnson.shiue@autodesk.com).

"Mirror Part" is almost equivalent to Derive Part -> with Mirror option. Another workflow you can try is to save the right-side part as a different part. Open the newly saved part -> Mirror Feature -> Whole Body -> check Remove Original -> OK. You will get the mirrored side of the body in an independent part.

Thanks!

[Anonymous]

Thank you all for the Info. What im running into is inside the mirrored component it already know it is sheet metal, (so i cannot convert) but it just gives me a solid to work from not any editable attributes on the tree.  Would somone mind showing me how to make this a fully editable normal part?

[Anonymous]

I found out that the LH was acting differently from the right because for some reason in the contour flange option inside "Edit Feature", the directional option although the same as the RH, was pushing the metal to the outside instead of the inside. I just reversed the direction and it worked, but I thought initially both parts should have had the same direction chosen, which I guess was incorrect.

[jtylerbc]

What you are seeing is exactly what you are supposed to be seeing in a mirrored part.  You're not really intended to edit it like a normal part - it just starts from the original source part.  They are linked, so any time you edit the original the mirror-image version will update to match.

As ccarreiras indicated, all you need to do is set the sheet metal thickness in the mirrored part.  Then you can create a Flat Pattern just like you would for a normal part.  I was able to flatten your mirror part without any trouble.

[Anonymous]

I was just able to do it reading everyones instructions now. Thank you all for the help, the only thing I don't like is not being able to edit the mirrored part in case I have a cut or something on the right I don't need on the left, but aside from that this will make a big difference in the prototyping in the future. Thank You all!

[jtylerbc]

You can to an extent - the derived geometry from the original part is a starting point for the new model, but you can add new features to it, pretty much like you would the normal part.

It's a little less straightforward to remove features from the original that aren't wanted in the mirror, but that can be done as well (Delete Face, Direct Edit, etc.).

[SBix26]

... and in Inventor 2016, you can use multi-body modeling in the Sheet Metal environment so that your right and left hand parts share as much or as little as you like-- add common features before the mirror, independent features after the mirror.  Derive to separate parts and unfold.

Sam B

Inventor Professional 2015 SP2
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