Hi, I am modelling a spot weld T-joint between two steel sheets. I was trying to use the CWELD function before finding out that the it does not work with free edge. The Glue connection gives a continuous connection between the sheets, so it may underestimate the strength of the spot weld joint.
I am wondering what is the best way to represent a weld joint, or more specifically a spot weld T-joint, in Nastran.
Solved! Go to Solution.
Well, you are mixing two words that are really opposed: spot welds & T-Joint welds. I do not see the way to perform a spot weldment unless the two plates are really parallel, please note a requirement to perform a spot-weld using CWELD/CFAST NX NASTRAN elements is the meshes you connect must be nearly parallel. To ensure this, the software projects two normals onto two meshes within the search distance. If the angle between the normals is greater than 20°, the NX AdvSim software does not create the connection.
In the following picture you have the classical weld joints, please post a sketch of your weldment to understand better your problem.
And here you are the classical spot-weld joint.
For pure spot welds I suggest to use the CFAST/CWELD Connection command to create NX Nastran CFAST and CWELD type connections in NX AdvSim. In NX Nastran, you use CFAST and CWELD elements to model connections, such as fasteners, spot welds, or rivets, between multiple sheet bodies. You can use CFAST and CWELD elements to connect elements either within a single FE model or between FE models in an assembly FEM.
Notes about CFASTS and CWELD connections:
Are not actual elements. They are simply connection definitions. NX Nastran internally generates the constraint equations that define the stiffness for the CFAST or CWELD connections when you solve the model.
Provide alternatives to traditional NX Nastran connection methods, such as CBAR, RBE2, or RBE3 elements or MPC constraints. In general, CWELD and CFAST connections are easier to create and use.
Here you re the typical aspect of a CWELD model I have just created in NX AdvSim V10 joining two parallel plates meshed with shell CQUAD4 elements using of spot-weld elements after a definition of an array of points:
Thank you so much for your detailed explanation, Blas. I was actually mixed up spot welding and tack weld. I would like to do tack weld on a Tee joint.
As far as I understand, CFAST/CWELD Connection command only works for Tee joint with 3D element mesh. For 2D element, the angle between two faces normal will become 90 degress. Is that right?
If that is the case, then how should I represent a tack weld Tee joint with 2D element mesh?
I also wondering was will be the difference between CWELD Connection, RBE and Glue Connection?
Thank you very much
Now I see what means "tack weld", searching in Google I see the image.
If this is your problem (always post a picture, an image is better than 1000 words!!) then the CWELD/CFAST command is not your command, here you can use the most simply method: manual merging coincident nodes at both ends, when meshing with 2-D Shell CQUAD4 elements this is possible to do it manually. If end nodes are not coincident, then you can use a rigid element RBE2 node-to-node.
The CFAST/CWELD CONNECTION command is the natural way to perform Spot welds between parallel plates meshed with 2-D Shell CQUAD4 elements. It has many advantages vs. the SPOT WELD command in NX AdvSim, for me the most important is that 2-D mesh not need to be coincident & aligned between both plates, you can have totally different meshed or element types QUAD/TRIA shell elements and the weld joint can be performed perfectly. To understand the differences feel free to play with both commands, make a simply model and you will realize the pros & cons. This is exclusive for NX NASTRAN users, in my opinion the best meshing approach for point-to-point spot welds.
Alternatively you can use Spot Weld command to define 1-D element connections by projecting a series of locations to selected faces that define the top and bottom of the meshes you are connecting. You define the points to project by selecting points or mesh points, or by selecting a curve or polygon edge and defining the mesh density along that edge. And you can joint not only 2-D mesh but also 3-D mesh.
The types of 1-D elements that Spot Weld command creates depends on the solver environment you specified when you created the FEM file. For example, in the NX Nastran environment, you can choose between different types of beam and rigid elements, such as CBEAM, CBAR, RBAR, and CGAP elements. In Samcef, you can choose between rod, beam, bush or rigid body elements.