Showing results for 
Search instead for 
Did you mean: 

NX Quick Tips: Product Interface Pt. 1 - Create WAVE Link and New Part


When you are part of a design team, rarely do you just work on one design from start to finish by yourself. Rather, you might create a design, and later your colleague will go in and do some additional work on it.  When that happens, they might encounter 4 or 5 different datum planes, axes, and CSYS to start from, not to mention all of the different bodies of geometry.  How will your colleague know which one to choose?


Product Interface eliminates the guesswork, because it allows you to define particular geometry selections. You have more control than if you were to use any kind of interpart associativity. Today, you will learn how to define a body, create a WAVE link, and design a new part in an assembly using Product Interface in NX.


Let’s start with how to define a particular body in your design. In this example, we have an aircraft body, and we are going to create a nose bulkhead to add to the assembly.


First, select the body you would like and change the selection type to datum. You see that the current setting is Allow Any, which means the user can select any geometry he or she likes. Choose the option Encourage Interface. This will issue a warning message any time the user chooses geometry other than that which you specified.


NX Product Interface select datum.jpg


Next, you should rename the interface to something more descriptive than the current generic Sheet Body. Let’s call this IML-ORG for Inside Mold Line and to indicate that this is the original geometry. Now there are two entries in the Part Navigator: the datum plane FWD NOSE BULKHEAD and IML-ORG. Notice how when you select one or the other, all of the associative geometry is highlighted.


Now, let’s create WAVE link associativity in the bulkhead to the front of the aircraft. Change the select intent to the correct datum and body. Note: When you choose the wrong datum or body, you get the warning message we set up in the previous step.  


NX Product Interface warning message.jpg


There are two associativity features embedded in this design. Use WAVE Interface Linker to grab on to the others. You can do so regardless of whether or not the part file is open or loaded. In this example, the file called Part Layout is already loaded. Grab the front end of the layout and use that as your associative information in your history. There is another file which, when opened, loads the properly defined product interface. Now, you have the cutouts and mounting with all associated info loaded into the feature history. You can start work on your design.  


First, choose the correct display part. We want to create a bulkhead as a forward design of this aircraft. Start by taking a section line based on the surface of the Inside Mold Line. Grab both that and the datum.


Once you have the inner section curve, you will create a solid body from there. Define the length and proper direction. Once that is complete, you notice the newly created geometry is not even with the rest of the design.


NX Product Interface uneven surface.jpg


Not to worry though; you can fix this quickly with Synchronous Technology. Using the command Replace Face, you want to replace the two outside faces so that they match the surface of the Inside Mold Line.


Next, hide the additional geometry so you can focus just on the part you will work on. You are going to clean out the shape to create a shell body, then define the proper thickness of the walls. Now that you have a good starting point, it’s time to go in and add more detail.


You see there are pockets and holes in the design that need to be removed. You can do so with the Extrude command set to Subtract under the Boolean setting.


NX Product Interface extrude holes.jpg


Once that is done, it is time to add ribs to this design. In this example, you have existing sketch curves that were previously defined in Product Interface.  Grab those curves and change the vector in order to extract that geometry to the predefined 6 millimeters.  Now, you can use Blend Pocket to clean out the remainder of the geometry.


Once that is done, you can see what the finished part looks like in the assembly. Simply remove the surface and reference sets, and display the part in the context of the assembly. 


Watch the video to see this process step by step! 


(view in My Videos)



Community Manager, Solid Edge
Become a Solid Edge Certified pro today!