is it possible to add thickness to a sheet metal part in one direction? i have a part i would like to rapid prototype to check fit but it is a thin sheet metal part, any ideas?
i need it in one direction but not the other, because something fits inside of it.
A thin feature has the attributes similar to sheet metal:
Thin Feature - One-Direction, Mid-Plane, Two-Direction
Sheet Metal - Direction or Reverse
Modify the thin feature
Why not change the model?
If not possible, add a surface to one side, thicken it.
If you want the part to maintain a uniform thickness the best way in general is to update the Sheet metal feature thickness. The sheet metal feature is basically a single direction extrude so the thickness will increase in one direction but how it effects your part and which direction will depend on how the part was modeled to begin with.
As a general rule you should try to design sheet-metal parts with features located and dimensioned so that the design is independent of the thickness. This will really depend on how complex the part is but I've designed a fair amount of parts that were prototyped in the US but manufactured in China so the design need to be made so the thickness could be changed from imperial to metric units without having to remodel the part.
If you want to just add thickness to an area where you think the part will not build properly or will be too weak I would suggest creating a new configuration and just add a little material though a basic extrude or as Chris mentioned create an offset surface and thicken it. .
i tried to update the sheet metal parts metal gauge, but that added thickness in both directions there for not fitting my part
The sheet metal feature only offsets in one direction. If it appears to be going in both directions you need to go through how each feature was created. Look for bends that are defined based on a line outside the part instead of inside. Specifically look at all the flanges and the Flange position. Default is what is show here with the bend being inside the line. If you want to make certain that the interior of your part is a spacific dimension you need to choose the second or third option.
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