Associative 3D FEA Models
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In this NX A to Z article, I will show you how to use Wave Linking and Synchronous Technology to make 3D finite element models that are parametrically linked to a CAD model.
Anytime you do a 3D finite element analysis, you either create the 3D CAD model yourself or you receive a 3D CAD model for your customer or maybe from another division in your company, etc. Either way, you start with a 3D CAD model.
If the 3D CAD model was created using NX, then making changes to the 3D CAD geometry and having those changes transfer down to your finite element model is an automatic and seamless process. If, however, the 3D CAD geometry was created in another system and was imported into NX, then an update to the 3D CAD geometry will most likely come in the form of a new file from your customer and therefore, a new import into NX. In that scenario, NX doesn’t know that the new imported part is a revision to the first imported part and therefore, NX will not recognize that much of the geometry is unchanged. Fortunately, NX has the ability to do a geometric comparison between two parts and transfer the links from the geometry in one part to the matching geometry in a new part. Even more, NX will allow you to decide if the links from the old part should be transferred to geometry in the new part that doesn’t match the geometry in the old part.
So, regardless of whether or not the CAD model was created in NX, you can link your finite element model to it so that changes to the CAD model automatically propagate to your finite element model, allowing you to update your meshes and rerun your analysis in a few clicks.
The Idealized Part and WAVE Linking
The key to this whole thing is setting up your finite element model and using WAVE geometry linking to make linked copies of the geometry from your CAD model in your finite element model. If you read the article on
Associative 1D FEA models, this will already be familar to you. Most of the setup is done for you when you create a new project in NX Advanced Simulation.
When you have part open and you switch to Advanced Simulation, you will see the Simulation Navigator. From there, you right click your CAD file and select
New FEM and Simulation as shown below.
This brings up the New FEM and simulation dialog box as shown below.
In this dialog box, you essentially tell NX what kind of analysis you are doing and what you want to analyze. At the top, it tells you it is going to create two files a .fem and a .sim file. The .fem is the finite element model – it has your meshes and materials. The .sim file is the simulation file – it has the loads and boundary conditions. The reason there are two files is because you can have multiple sim files using the same fem file. There is also a third file that you have the option of creating and that is an idealized part file. The only time you don’t create an idealized part file is if the geometry in the CAD file was created exclusively for meshing. So because we received our file from a customer and we need to make some changes to it before meshing, we are going to create an idealized part. Notice the idealized part file as the extension .prt – in other words, it is just a normal NX file; however, you must have the lowercase i before the extension so that Advanced Simulation knows that it is an idealized part. Using these three files allows you to have multiple idealized part files linked to one original part file, multiple .fem files linked to one idealized part file and multiple .sim files linked to one .fem file. This minimized the amount of work necessary to run different analyses on the same part.
So when you click
OK in the New FEM and Simulation dialog, NX is going to create the idealized part file, the .fem file and .sim file and then open the .sim file and open the Solution dialog box for you to configure the analysis that you have chosen to run. We’re not interested in the .sim file or the Solution options at this point, so cancel the Solution dialog and if you expand everything in the Simulation Navigator you should see something like what is shown below.
At the top is the .sim file and then the .fem file and then the idealized part file and then our original 3D CAD file. Under that is the Polygon Geometry, which is what NX converts the original 3D CAD geometry to in order to mesh it.
Before we can mesh our part though, we need to simplify it. We need to get rid of blends and maybe some small holes, etc. This is where the idealized part comes in. If you right click the idealized part and make it the displayed part, you can switch to the Assembly navigator and see that your idealized part is just a regular part file with your original part file brought in as a component. This is shown below.
So, the idealized part file is just a regular assembly file, but we need to make changes to the component at the assembly level without affecting the component. This is where the WAVE Geometry Linking comes in.
When you first switch to the idealized part, NX will tell you that you need to create a WAVE linked body to do any geometry simplification. I would show you the message, but I told NX that I didn’t need it to tell me that anymore. So, to create a WAVE linked body, click the
WAVE Geometry Linker button (be aware that the
Synchronize Views button looks the same).
Body from the
Type menu and then select the component you want to analyze. If you have multiple components that you want to analyze, just select them all to create linked bodies of all of them.
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.
This method of using the assembly functions and WAVE Geometry Linking to provide an editable linked copy of the original part without effecting the original part is called the Master Model Approach. It also applies to CAM and Drafting and any other applications that happen downstream from modeling. Using this approach allows you to have the control that comes with maintaining a single source for your part definition while also having the flexibility of having multiple editable copies of your 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.
Simplifying the Model
Now that you have your linked body in your idealized part, you have a couple of options for geometry simplification. There are some tools specific to Advanced Simulation and there is also Synchronous Technology along with the entire NX CAD modeling toolset for that matter. For deleting blends and holes, you can used
Idealize Body from within Advanced Simulation or you can use
Delete Face. One advantage to
Idealize Body is you can delete all the blends under a specified size; however, the Synchronous
Delete Face command gives you access to more sophisticated selection filters.
In addition to geometry simplification, you may also need to add some lines and points to place concentrated masses in the model. This kind of stuff can all be done in modeling. Finally, you may want to extract midsurfaces if you want to do any 2D meshing.
The great thing about all of these commands is that remain parametrically linked to the original CAD geometry through the linked body.
Let’s say for example that you just want to delete all the blends in the part. First you use the
Idealize Body command as shown below to delete all the .030” blends.
Then you can use the
Delete Face command to delete the blends between the bosses and the arm as shown below.
Now, the designer decides that they need all the blends that were .030” to be .045” and the also need to make the whole part smaller. If the designer is using NX, then after they make the change, you just open the part and you see that the delete face command is still intact, but all of the faces that were deleted by the Idealize Body command have now returned. So, open the Idealize Body command and change the Blend size to .050” and you’re back to where you were in just a couple clicks. If you had meshes in the FEM file, they would update automatically. If you had done any splitting or midsurfacing, they would all update as well.
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. So you get your new customer file, import it into a new NX file and then inside your idealized part, delete the assembly component that is your original part. When you do that you’ll get a message saying that you are going to be breaking the link as shown below.
Just close the message and then add your new part to the idealized part as an assembly component and you will see the new part on top of your linked body (the new part is orange).
Now you have to tell NX that your linked body needs to be the new part, but you don’t want to have to redo all of your edits. So, open up the linked body and select the new part and then click
Geometric from the
Matching Algorithm menu and the click
Find Geometric Matches.
NX found 217 matching faces and they are shown in Yellow.
The other faces do not match, so you have a couple of options. First, you can increase the
Deviation Tolerance. The danger here is that you might find some faces that don’t actually match. Then after that you can manually select matching faces. I increased the
Deviation Tolerance to .050” and got some faces that didn’t match, so I started over and went back to .030” and got everything except the bosses.
Synchronize View is selected so the two views will move together. Now, you can manually select the remaining faces, so make sure that
Manually Define Matches is selected in the
Current Activity menu and just pick a face on the left and a matching face on the right and click the
Add New Match button (once you do this once, you can use the middle mouse button to add a new set).
Once you have matched all the faces, click
OK and you’ll see that all the work you did to simplify the original part has now been carried over to the new part.
That’s it. Hope you learned something.