One of the potential clients that I encountered ask whether Solid Edge has the capability to simulate weld strength (while we can mark assembly as weldment and apply weld, those probably would not contribute anything to the result)
I know that some softwares (*cough cough SW*) has a weld connector to connect 2 components in assembly together. Does solid edge has such function....?
Solved! Go to Solution.
I have a feeling [probably wrong though] that this is available, but only in SE-Premium, as it has the more full "Simulation" package, as opposed to Simultaion Express available in SE-Classic.
Design Manager Streetscape Ltd
Solid Edge 2019 [MP5] Classic [x3 Seats - Cloud Enabled]
Windows 10 - Quadro P2000
Nope. Only glue connector is available. This is taken from the Simulation tab bundled in SE-Premium
Now where do I file in an enhancement Request
Yes this is possible to do in SE (premium license only). You have to use manual connectors to connect the sides of your weld bead to the parts that are welded together. That way your parts are connected to each other only via weld bead. Here's a video how:
That is certainly one of the good approach to simulate welding condition. My only question will be is...will this be a good approximation to simulate real time weld condition?
and does it behave like CWELD connector of Nastran solver?
The CWELD element of the NX NASTRAN solver is used in general to define SPOT WELD connections, and is not supported in SolidEdge ST8 SIMULATION, only in FEMAP.
The CWELD element let you establish connections between points, elements, patches, or any of their combinations. Although there are a number of different ways to model structural connections and fasteners in FEMAP with NX Nastran, such as with CBUSH or CBAR elements or RBE2s, CWELDS are generally easy to generate, less error-prone, and always satisfy the condition of rigid body invariance.
Basically, for all connectivity options, the CWELD element itself is modeled with a special shear flexible beam-type element of length L and a finite cross-sectional area which is assumed to be a circle of diameter D, according the following picture.
Here you have a picture with the different options we have to define a connector using CWELD elements: the main advantage is that meshes not neet to be congruent using the PATCH-TO-PATCH method.
In the FEMAP interface we have full capability to define CWELD elements for the NX NASTRAN solver. To learn more take a look to my blog in the following address (video included!!): https://iberisa.wordpress.com/2012/03/05/elementos-cweldcfast-en-femap-y-nx-nastran/
And this is the typical application of the CWELD elements: spot-welds connections between 2-D Shell elements!!.
Regarding the question of how to joint weld components in SIMULATION, well, the preferred method is to use the GLUE surface-to-surface connectors, either manually or automatic commands: in the manual method the user select explicitely the SOURCE & TARGET solid faces or surfaces (my recommended method!!), meanwhile in the automatic command is the software who search for surfaces or solid faces to define the connector in base of a maximum GAP distance specified by the user.
GLUE surface-to-surface is a simple and effective method to join meshes which are dissimilar. It correctly transfers displacement and loads resulting in an accurate strain and stress condition at the interface. The grid points on glued surfaces do not need to be coincident. Glue creates stiff springs or a weld like connection to prevent relative motion in all directions. Please note that the internal "glue elements" are created by the NX NASTRAN solver from glue definitions during the solution, OK?.
But this is simply a meshing approach, the correct procedure to use depends of what the end user really need to calculate: welds are really, really complex, and in general BUTT-joints or T-Joints are not meshed in detail in the FE analysis of the full structure, the resulting FE model will have millions & millions of nodes, impossible to solve!!. We capture the mission of the seam weld that is to joining rigidly two bodies, then we can simply "merge" nodes between plates or Shell elements, or use GLUE surface-to-surface contact between parts of the assembly.
Another history is when a local fatigue analysis is required to perform in the seam weld, then a different approach is followed, we need to mesh in detail the weldments and use specialized fatigue tools like winLIFE integrated in FEMAP to take advanced of stress results computed by NX NASTRAN:
The real structure is modelled by 2-D plate CQUAD4 elements (weld stiffness is not taking into account) or 3-D solid CHEXA elements, here including the seam weld. The size of the 3-D solid elements should correspond as minimum to the thickness of the plate to achieve a finite element model with a limited number of elements, but the recomendation is to have three elements in the thickness. The arrows, including the circles in the figure, show the points from where the reference stresses (replacing the strain gauges) are read. The extrapolation to the weld toe in the case of 3-D solids (b) respectively to the plane in the case of plates (a) must be carried out by the user (we run macros in FEMAP to to the task).
In the case of 2-D Plates we can use different meshing approaches: either use of RBE2 rigid elements, or capture the weld stiffness using Shell elements locally.
Well, etc.., as you see this is a complex matter and require specialized actions and manage dedicated software tools.
I only wanted to explain the CWELD element of NX NASTRAN ....
...in general BUTT-joints or T-Joints are not meshed in detail in the FE analysis of the full structure, the resulting FE model will have millions & millions of nodes, impossible to solve!!...
Jumping into this thread, we are trying out a temporary license of SE Premium to use the Simulation package as a design tool, particularly for weldments (currently using ST7). Preliminary testing of fillet welds using the glue weld connector shows significant variation in results from textbook hand calculations due to hot-spots. The FE model meshes and solves, but results vary considerably.
Understanding that we don't have or need FEMAP/specialty software required for detailed analysis, is there a standard workflow for using Simulation and refining weldments to get ballpark stresses in and around welds so we can speed up our design cycle times before sending out models for detailed analysis?
For those of you who use SE Simulation to design weldments, in what ways do your simulation models differ from your production models? Besides simplifying holes, do you use apply fillet welds and use glue connector, or do you use a different workflow?
Thanks in advance.