Element birth and death in Abaqus Implicit

[anoop_1989]

Dear all,
I am doing a welding heat transfer analysis in Abaqus. Can anyone suggest how to include the element of birth and death in Abaqus implicit?

 

[Erik Panos Kostson]

Some members have suggested the Abaqus Welding Interface plugin, have a look at that, becuase it does a lot of clever things.

See this video also:

https://www.youtube.com/watch?v=OB8CzFHTnzA

 

[FEA way]

In Abaqus this is called element activation. There's a predefined subroutine for it called UEPACTIVATIONVOL. Keyword to specify elements for activation is *Element progressive activation while keyword to turn it on or off is *Activate elements.

 

[Erik Panos Kostson]

@FEA way. You sound like you have used this FEA way, can you give an example of how it is used, it is all very abstract and very difficult to use this for anything - I think that would help anoop_1989

 

[FEA way]

I used these techniques but for a little bit different kind of analysis - additive manufacturing process simulation. However the procedure should be very similar. I suggest reading the documentations chapter regarding this type of analyses. There are even some examples in Example Problems and Verification manuals.

 

[Erik Panos Kostson]

What chapter in the documentation do you refer to?

There is also an AM plugin (scroll down to the bottom of the link and to the section on downloads):

https://www.3ds.com/products-services/simulia/trends/digital-additive-manufacturing/

I think though the welding one is more suitable for you (think you did something with welding)

 

[FEA way]

I don't have access to current documebtation (it's a new functionality) but I think it's called Additive Manufacturing process simulation. There are also additional chapters for specific options. The most interesting example in Example Problems manual is titled "Coupled thermo-mechanical simulation of a laser powder bed fusion process".

Be very carfeul with this plugin. I've found out that it may not work properly. It will be better to modify inp file manuall and add necessary keywords.

 

[Abaqus_FEM]

Maybe you don't need to consider element birth/death in your simulation at all. You could model the weld bead as a part in the beginning of the simulation but prohibit any interaction with the rest of the model via GAPCON and FILM subroutines until the torch has passed. Here's a short document. It doesn't go into detail how things have been done, though.

Link

This is just an idea, since I don't know the exact problem you are working on.

 

[anirudh123]

anoop ,
I am also doing simulations in AM. Right now i am stuck with the UEPActivationVol. First of all where do we link this subroutine in abaqus. If possible please guide me through this process.

 

[FEA way]

Which version of Abaqus do you use ? In newer versions AM process simulation capability was significantly improved. This also applies to AM plug-in which now works really fine (some modifications to .inp file usually have to be done though). The plug-in will automatically apply element activation to your analysis. But if you don’t want to use it you can still easily apply element activation since in newer versions of Abaqus this subroutine is built-in. Exemplary input file can be found in the „Coupled thermo-mechanical simulation of a laser powder bed fusion process” chapter in the documentation. There you can also find a simple verification problem that compares partial and full activation.

 

[anirudh123]

@FEA way
thankyou for your response.
I am using abaqus 6.18.AM plugin is not available in my software may be because i am using an institute subscribed package.
If i want to use the UEPACTIVATIONVOL subroutine where should i access to link up with the subroutine like for example DFLUX is been used with LOAD and is uplinked while defining the job.

 

[Joachim_S]

@FEA way
Glad to find somebody with experience in AM process simulation! Could you please tell me where to obtain the AM plug-in? We run Abaqus 2019, so it should be compatible to our system. Where in the Abaqus documentation is the „Coupled thermo-mechanical simulation of a laser powder bed fusion process” example? I could not find it in the "Example Problems" section nor in "Verification". Unfortunately, our online documentation does not have a search functionality, because the Exalead database is not installed yet.

 

[FEA way]

AM plug-in can be downloaded from Dassault Systemes Digital Additive Manufacturing webste. I don’t give link because it can’t be downloaded directly. You have to find Download section and select Abaqus/CAE Plug-In. Then you will be redirected to form where you have to provide your email and company data if I remember correctly.

This chapter of the documentation can be accessed if you select 2019 version and expand Example Problems. There’s a section for AM process simulation. In the documentation there is also information about these analyses including details regarding built-in subroutines.

 

[Joachim_S]

@FEA way
Thank you for your advice! I have been able to download the plugin from

https://www.3ds.com/products-services/simulia/trends/digital-additive-manufacturing.

I Unzipped its contents to ...\CAE\Plugins\2019, and an entry "AM Modeler (show/hide)" appeared in Abaqus CAE's "Plug-Ins" menu. To find the corresponding chapter in the Example Problems documentation was a bit tricky, because it does not seem to exist in our local documentation (even though this had been updated just yesterday), but only in the version of the documentation that is provided directly by help.3ds.com. Surprisingly, the two documented examples only use Abaqus/Standard, and so they don't really help with the CAE plug-in. Do you know any other set of example files (capable of running) that supports Abaqus/CAE?

 

[FEA way]

Unfortunately documentation examples only feature downloadable .inp files, without .cae models. I don't think there are any other sources where you can find .cae files for AM process simulations (since it's new capability in Abaqus and not as popular as other types of simulations). However you can recreate this example from the documentation in Abaqus/CAE. In order to do it merge input files containing definitions of nodes and elements into single input file. Next import it as an orphan mesh to Abaqus. Use Geometry Edit --> Faces --> From element faces to recreate geometry (it's rather simple in this case). Position the parts in Assembly, define features described in the documentation (materials, steps, interactions and boundary conditions). Then start the AM plug-in and define remaining features as provided in the example (some settings may not be mentioned in the documentation so examine the input file). Be careful - when you generate the .inp files from plug-in review them carefully and compare with those from documentation because for sure there will be some differences (plug-in omits some features and has different default settings than you would expect in case of this example).

 

[Joachim_S]

Oh, my! This is going to be quite some work. As a first step, I simply used CAE's job manager to run the input decks, but even that will take days of pure runtime. Apart from that, it'll take me some time to understand that strategy of running a heat transfer analysis for an extremely long time period, discretized in thousands of time increments, followed by a huge static job, again in thousands of increments. I would have expected to find the two analyses interlaced incrementwise...
However, your elaborate instructions have already helped me quite a lot! When merging the input files, would you recommend to add the file ABQ_am_special_purpose_types.inp as well before importing the merged file to CAE?

 

[FEA way]

Unfortunately solving this example will take a while (few hours for sure) but it’s advised to omit CAE (it requires additional computational resources) and submit the job through command window (type abaqus job=input_file_name interactive cpus=number_of_available_processors). You can even use sequential submission so that the static analysis starts right after the first one ends - just create .bat file with proper commands.

Mesh in this example is indeed very detailed and there are many increments but one of this method’s advantages is that it can solve the same problem with coarser mesh and less increments maintaining very good accuracy. Give it a try.

No, you don’t have to include this file. AM plug-in will implement calls for necessary built-in subroutines to generated input file. So you only have to import mesh.