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NX 11 Flattening and Forming


Oftentimes in certain industries—say, aerospace, for example—you face the challenge of having to apply geometry to complex surfaces or shapes that are not well-suited to traditional workflows. The new Flattening and Forming command in NX 11 makes it easy, allowing you to work with freeform surfaces and shapes just as you would wrap and unwrap cylinders or cones. Read on for a step-by-step guide to using this command as we walk you through an example.


flatten and form nx 11.jpg


To start, we have a freeform swept surface that represents the side of an aircraft to which we would like to add some portholes or windows. The caveat: The windows can only be added while the surface is in a flattened state. So, we must flatten the surface, make any changes, and reform the surface so that those changes are then applied to the original shape.


Open the Flattening and Forming window and select Flattening from the dropdown menu underneath Type. Next, select the surface you want to flatten. You specify an origin point—in this case we will pick the corner—then choose the direction in which you want to flatten the surface.


 flatten and form 2 nx 11.jpg


Now that you have a flattened surface to work with, you may wonder just how accurate the flattening tool really is. Luckily there are reporting tools that allow you to go in and check. Open the Flattening and Forming window and go down to the bottom where it says Distortion Map. You can select what specific type of distortion you would like to show: none, length, area, or angle. In this case, we are going to select area.


Now we see the areas of deformation indicated by a range of colors—from red having the highest level of deformation to blue with the lowest. This gives an idea of how accurately this sheet has been unfolded.


flatten and form 3 nx 11.jpg


The Distortion Map is purely based on mathematics (unlike similar CAE tools that are physics-based) and employs the perseveration of area method to determine the levels of deformation.  It’s as if we were to break the model into finite elements, map those elements down onto a flat area, and then minimize the changes between the two.


Let’s go back and add a curve to the model, which will act as a guide for us later when we apply a pattern to the surface. Select an isocline curve and set the angle at 0 degrees. Next, select the surface and specify the direction. Go into the Part Navigator and drag to reorder the curve, bringing it in front of Flattening.  Now when you edit the Flattening, you can add additional objects such as the curve we just added.


In Flattening and Forming underneath Transformation Objects, choose Select Objects and pick the curve you would like to map down onto the surface. Select OK to apply the changes.


Next, go into the Sketcher. Select the face you would like to modify. Using the Circle tool, create and place a circle. Return to the Home tab, and select the Pattern Geometry tool under Pattern Feature. Select the geometry and specify the path—in our example, that would be the circle and the curve line respectively.  


flatten and form 4 nx 11.jpg


Now we have the circles on our flattened sheet but how do we transfer them back onto the formed surface?


Reopen the Flattening and Forming window, and this time we are going to select Forming and Reuse from the dropdown menu underneath Type. Pick the object that was flattened, along with any additional features you would like—in this case, the circles we just added—and we see now that those are mapped back on to our original surface.


Select Trim Sheet in Surfacing to open the Trim Sheet window. Select the sheet and objects to trim, and then select OK to complete the command. Now we see that our modification is finished, and the aircraft body now contains portholes.


John Baker demonstrates this workflow in our latest NX Quick Tips video, which you can watch here.  


(view in My Videos)

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Hi @AmyReyes 


Thank for your sharing!


which NX licenses provide access to the Flattening and Forming tools?