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Synchronous and WAVE in NX CAM
In this NX A to Z article, I will show you how to use Wave Linking and Synchronous Technology to make CAM files that are parametrically linked to a CAD model.
The Master Model Approach
Something that is talked about a lot with NX is the Master Model Approach. What this means is that the NX file that contains the 3D model of your part is the Master Model and this file is the only recognized authoritative source for the geometric definition of your part. That being the case, you want to limit the contents of the file to only the 3D model of the part. So then how do you use the 3D model of your part to create the CAM programs and prints and the finite element analysis model? The answer is Wave Linking and Synchronous Technology.
From a manufacturing standpoint, a typical scenario is you receive a CAD file (either NX or otherwise) from a customer or from the engineering department in your company and you need to create the program(s) to machine the part. You could just open or import the part and start programming it; however, seeing as how the file you received may be the only source for the geometric definition of the part, it isn’t a good idea to do your programming inside the file, so you want to use the Master Model Approach in order to maintain the integrity of the original 3D CAD model. The Master Model Approach is actually very simple – you create an assembly for every secondary file associated with your Master Model. So every drawing, every CAM file, etc. is an assembly file with the Master Model added as a component. Once you have the Master Model added as a component, you use WAVE Geometry Linking to create an associative copy of your Master Model in the CAM file and then you can use Synchronous Technology to make changes to your Wave linked copy that may be required for manufacturing without affecting the original Master Model. Furthermore, you can use this approach to create multiple CAM files if necessary and they will all be working from the same Master Model.
Assemblies and WAVE Linking
There are a couple ways to implement the Master Model Approach for an NX CAM file. The first method is to create a new blank NX file and then bring in the Master Model as a component from the Assemblies menu and then start the manufacturing application and select a CAM setup. The other way is to create a new file using a CAM template that is preconfigured to implement the Master Model Approach. If you create a new NX file and select the Manufacturing tab, you will see a list of templates as shown below.
The thing to note about this dialog is the Part to reference section at the bottom – this is where you specify your Master Model. If you already have a file open, NX will assume it is the Master Model and add it as the Part to reference, but you can select any file.
So, select the CAM template that you want to use (For more on CAM templates, check out this NX A to Z article) and NX will create an assembly file and bring in the part you selected as the Master Model (the Part to reference box) as an assembly component as shown below.
Now, you have your CAM file created and your Master Model in your CAM file, so the next step is to create the Wave Linked body. Tto create a WAVE linked body, click the WAVE Geometry Linker button from the Assemblies menu.
Then select Body from the Type menu and then select the Master Model as shown below
Now if you switch to the Part Navigator, you will see you have a Linked Body. The name comes from the name of the body in the original part.
The next step is to change the color of your linked body so you can tell it apart from the original component. So, hide the component and then edit the display of the linked body to change the color. You’ll notice when you hide the component that there is no change in the graphics window because the linked body is the same color and is in the exact same location.
The point behind WAVE Linking is that it gives you the flexibility of having the Master Model CAD geometry inside your CAM file as if you had created it there without compromising the integrity of the Master Model. The only difference between the linked body and the original Master Model is that there is no feature history with the Linked body. Without Synchronous Modeling, this would make the linked body very difficult to manipulate, but with Synchronous, it is as easy if not easier than editing the original Master Model. The Synchronous Modeling toolbar is shown below.
Let’s say for example that you want to delete the holes from the part in your CAM file because they are put in during a different operation, just click the delete face button (the third from the right) and select all the faces for the holes and click OK.
The Synchronous Modeling tools allow you to move faces, delete faces, change the size of blends and holes, add adjustable dimensions to the Linked body that control the size of its features along with many other capabilities. If you have NX CAD, then you also have the entire NX CAD toolset available to make changes to the linked body.
So now that you have your Linked body exactly how you want it, switch to the Geometry View of the Operation Navigator and open the Workpiece and select the Linked Body for your Part Geometry. You would add the Blank geometry as a component as well if you have a Master Model for the blank geometry. If not, you can model it in your CAM file or use the Autoblock command. You can also use the resultant In Process Workpiece from another CAM file if this program is not the first program done on the part.
The other great thing about Master Models and WAVE linking and Synchronous Technology is that you can choose to have your Linked body either update automatically or manually whenever the Master Model changes. Furthermore, any of the changes you made to the linked body will stay intact provided the underlying geometry is still in the Master Model and all of the CAM programming that you do will also automatically update to reflect changes in the Linked body and therefore the Master Model.
That is all well and good if the designer is working in NX, but what if you received a revised file from a customer in the form of a STEP file or parasolid. In that case, NX is not going to know that it is just a modified version of your original part, so you have to use the WAVE Replacement Assistant to tell NX that it is the same part with just a few modifications. To learn more about how to do this, check out the NX A to Z article
Associative 3D FEA Models and scroll down to the section on the Replacement Assistant.
That’s it. Hope you learned something.