I want to extrude the sheet metal body, with out changing the sketch dimension , for example i have 100*100 sheet body ,now i wish to extrude the length of body. There is any option we have like extrude ,. presspull to extend the area of sheet.
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The extrude command lets you select the external edges of the sheet to define a solid body (use the 'Sheet Edges' selection intent filter). However, if you intend to use that extruded shape as the base of a sheet metal part (e.g. to add flanges, etc.) you first need to use the convert to sheet metal function on that extruded shape before you can add the secondary features.
You can still use general Modeling App commands such as 'Offset face', 'Offset Region'.
Besides, Those commands do not make problem to 'unbend' or 'Flat Solid'.
(Generally, to design complex sheet metal part, you may switch 'Modeling' and 'Sheet Metal' App.)
You have posted a number of questions about sheet metal recently. I would encourage you to go through the learning material available from Siemens on this topic.
A few comments on the replies above.
To extend the side edge of a sheet metal body. Although using unite as shown by @Abeinjapan works and is a valid workflow, extrude may not be appopriate in all cases. I would use the tab command.
Either edit the original sketch and extend it that way or add a 'secondary' tab feature The value here is you can create additional profile shapes that you need later in the design process.
The die and punch functionality is explained above using the solid punch command.
I would not recommend using synchronous technology commands such as offset face or offest region as suggested by @SKAHN. Although it works in most situations, it can cause issues for sheet metal functionality. A good rule for a robust and reliable model is try and only use the commands within the sheet metal application until you become more experienced.
Finally, I would recommend upgrading to the latest release of NX you can, there have been numerous improvements since NX8.5 that has been out of maintenence since 2015.
Continue to reach out here and also take a look at the NX-Sheet-Metal Group in this forum
You can also hop over to the modeling environment and stretch the edges with Synchronous; Move Face; Pull Face; Ofsett Region, etc...
One warning though:
Synchronous tools can also invalidate the sheet metal model;
e.g. when you change a thickness or alter an inside bend radius without maintaining the outside bend radius concentricity. To name a few.