Hi to all.
I share with you guys some of my research on welding simulation using nx 10. This begun because somebody said that just Sysweld and Simufact software are able to get well results, I´m not agree with that. Please nx fans could give your opinion? I have to say that I´m new with nx nastran.
So...Have nx nastran some tool to simulate from an easy way this kind of problem ? Because my simulations are very simple but it's very time consuming, and I would like to increase the frame of work to a bigest body. For example, i would like to learn how to set a formula on time and length domain and whether nx nastran can use death mesh and born mesh to simulate filler metal depositions.
Please, sorry for any grammar mistake english is not my mother language.
Thanks to all....!!!
NX Nastran should be able to solve this problem using the advanced nonlinear solver (solution 601). That solver is primarily used for statics solutions, but it also supports thermal and coupled thermal-mechanical solutions. The problem you will run into is setting up the solution as the thermal portion is not supported by NX pre-processing. Solution 601 is best for your solution because it supports element birth/death over time. There is also solution 401 which was first introduced in NX Nastran 9. It can be coupled with NX Thermal for coupled transient nonlinear thermal-mechanical solutions. Solution 401 does not yet support element birth/death though. This solution is ideal for you in terms of pre/post processing, except that it is missing element birth/death.
The loading aspects of your analysis could be done with either solution and are supported by NX pre-processing. Spatial-transient loads are supported through fields. Please review the NX online help regarding the use of fields to define spatial and time varying loads.
I’m glad to read your opinion about it. For instance, I was running NX thermal/flow solver (thermal advance solution) and mapping temperature onto structural analysis 101, this is one-way physical solution and it’s pretty simple (static analysis). Then I tried with NX thermal 159 transient solutions gotten better approximations for thermal field when domain has geometric complexity, I don’t why.
But the main problem that I´m having is to get temperature from transient analysis and mapped to structural solution for the time step that I want. Here there is the error message. It would because there is duplicate nodos in the mesh, I’m using node merge tool before thermal analysis but then nx is considering the mesh is completely the same geometry, if you may see above I’m doing geometric division for filler metal depositions, so I need to use different volume, before and next differential volume has to share the same face. How can I solve this?
So, the work flow I’m using is… creating field table from the .op2 thermal result file and mapping this temperatures in to structural solutions, the new thing is that I will use solver 601 like you suggest. Please, what do you think about this work flow?
Also I have no access to 401 solver licensing. What about with NX multiphasic, can do this?
You get the duplicate lookup value because the field creation is trying to write two different temperature values for the same Cartesian point locations where you have coincident nodes. Alternatively you can create a Node ID table. With a node ID table, it won't matter that the points are coincident because all of the node IDs will be unique. Using a node ID table assumes that you are using the same mesh for the thermal and structural analysis.
If you have different meshes, then you will need to create different fields using separate regions and the Identify Results command. Identify Results lets you query the results based on groups, meshes, area selection, etc., so you would choose nodes in Identify Results that aren't coincident. Then use the option to create a field from the Identify data. Repeat the Identify Results action for each unique region that you need a temperature field for. Lastly, you would define temperature loads on each region using the appropriate field.
Thanks a lot for you help. I´m able to get result using node ID like you suggest but I don´t know whats happening with the new field created, appears into table file below campus but when I go to map temperature using a new temperature load I can´t select the new table that it was created, (node id table) it is empty ¿? Please, sorry for so many questions.
I will try with NX Multiphisic, I didn´t used because I was running one way thermo-mechanical analysis, but if you believe this may be the best choice, I will.
Thanks again Mark
Regarding related posts, this one has grabbed my attention. I have also a question regarding the weld analysis which I'd really appreciate wether you could help. According to some normative, there are some simplified checks to validate the strength of a weld based on the efforts along the welds.
So far, I've stitched the edges of the shell meshes to simulate the welds and ease the simulation but this hassles the extraction of the loads along the weld: one solution would be to sum up all the stresses along the edges (their nodes' values), rather tedious and cumbersome. Would you know another less time-consuming approach.
Thank you in advance,
Your question gets into durability methods relative to the weld. I don't have a lot of experience with durability, but generally the basis is various forms stress/strain data like principal stresses. You could take your model a bit further by including the width of the welds in the meshes. For the welds that you point to in your image, the width isn't much more than the plate thicknesses. The width of the weld at the base of the vertical plate as it connects to the horizontal plate could be more. Then you could also assign specific materials to the weld meshes that represent the weld material. Now you'll have more accurate stress data as the basis for durability calculations.
as Mark already mentioned this is typically handled in strength and durability of the welds. The trick is indeed how to get from results of relatively simple meshes to good stress values of the weld. There are several approaches to this. The more traditional (nominal stress, hot spot, etc..) is to take stress values away from the weld line and extrapolate the stresses into the weld. These approaches are typically quite mesh dependent. A better approach is to take the load flow through the connection (i.e. the element-nodal forces and moments) and back calculate the stresses in the weld using information on the real weld structure. (See e.g. https://doi.org/10.4271/2013-01-1008 for details).
These methods today are implemented in the Siemens LMS Virtual.Lab durability tools (and working with results of stiched welds from Simcenter), but of course will also come to Simcenter 3D.