Time-dependent Co-ordinate System 4

[Matthew_19]

Hi Everyone,

I am a novice modeller looking to seek help using ABAQUS. I currently have a FORTRAN subroutine that models the laser heat source but I am struggling to move the source to exact locations across the surface, a colleague mentioned to me about using an excel spreadsheet that had time-dependent coordinates that ABAQUS could read, maybe implemented into the subroutine and the laser would move to each location via reading the coordinates file previously written in excel or similiar. Can anybody recommend tutorials or help with how to move a heat source across a surface/body based on X, Y and Z coordinates and how to make sure ABAQUS reads the file?

I would want the laser to start at a location, travel along the z-axis then move slightly down the x-axis by a known distance then repeat the scan? Etc and so on.

Many thanks

 

[FEA way]

Yes, the plug-in should define everything. In some cases it is necessary to make small changes in the input file created with the use of AM Modeler but in this case it shouldn't happen.

Do you have the text file with nozzle path prepared ? That's the first thing to do, before using AM plug-in. Power should be defined in this file as well. There's no need to define full path already, you can start from short file first. Here's an example in SI(mm) units:

4,0,0,0,100000
8,0,0,5,100000
10,0,3,5,100000
16,2,3,5,100000

Here the nozzle starts from (0,0,0) at analysis time t = 4 s. Then it moves 5 mm in +Z direction. This motion takes 4 seconds. Next the nozzle goes 3 mm in +Y direction. This destination is reached at t = 10 s. Finally, it moves 2 mm in +X direction and reaches the target at t = 16 s. Laser power is constant all the time and equals 100000 mW.

The plug-in allows you to plot the toolpath defined in event series on your model so that you can see how it looks like.

When you finish defining AM analysis you have to submit the job as normally done (using CAE or command line). Keywords provided by the plug-in will be automatic added to your model's input file.

 

[Matthew_19]

Hi FEA way,

I understand your example, very well defined and makes sense. If i were to write out the nozzle path, (which is the exact same as the deposition path) would you be able to show me how you put this through the CAE plug in, I am just unsure of all these "event series" and what to include in each series. I would like to see how the toolpath looks on the model via event series, as you mentioned but unsure of how. In the next post I shall attach all my variables and CAE file. Thank you very much for the help, I wish there was a CAE example to follow, as I am very confused by the amount of tables.

 

[Matthew_19]

Problem described:

CAE is attached with all geometry, meshing, material properties, steps (heating and cooling) and so on. I previously tried to write a subroutine in FORTRAN but now deleted the load and made a uniform as I think that would be the case since you define this in the AM section.

Geometry of substrate part is X(0.12) x Y (0.01) x Z (0.1) all in metres
Geometry of deposit X(0.0054) Y (0.005) Z(0.1) to be deposited in centre of build
Ambient temperature 25 degrees celcius

I want to deposit a laser path:
Double Goldak deposition
Power = 700W
The absorption ratio is = 0.35 (Would this make a total power of 245W) does 35% efficiency seem right? For laser metal deposition
Travels at 10mm/sec (10 seconds per deposition)
Cooling time 2 seconds between each deposit line
1.8 mm between each deppsotion 3 layers
0.5 mm between each layer 10 layers

Want to apply radiation and convection (radiation = 0.4 emissivity, to ambient 25 degrees)
Convection (10W/m/degree) to ambient temperature 25 degrees

Bead thickness = 2 mm or 0.002m
Sep over = 1.8 mm or 0.0018m

So for only the first layer, (I know the Y coordinates would go up in 0.5mm between each layer for deposition path) the time nozzle path prepared is attached. Hopefully it makes sense, I have made the top left corner the start datum (0, 0, 0)


I am unsure whether the power goes on during cooling or to remove it also..

I hope everything else is attached and you can see and makes sense, thank you very much for this, I am very unsure of the "event series" "tables etc"

 

[Matthew_19]

and the cae file - FOR INCONEL 718, all units in M (material property and geometry)

 

[Matthew_19]

Please note, it's not a sequential thermomechanical model yet, only transient heat model - not sure if this makes a difference but doesnt include strength etc properties - only themophysical

 

[Matthew_19]

laser spot size radius = 1mm
penetration = (assumed)1.1 mm
want to model as a circular source therefore cf and cr = 1

 

[Matthew_19]

When you submit the job.. would you need to compile all the files into one document or would it already be compiling them from CAE file?

 

[FEA way]

I prepared the .inp file for your model. You can find it attached to this post. I don't share .cae file because I use newer version of Abaqus so you wouldn't be able to open it. Furthermore, I made some changes directly in this file after it was generated by the plug-in. Please check the settings of "ABQ_AM.MaterialDeposition.Bead" Parameter Table because I'm not sure if I understood your bead size data correctly.

To set this in AM Modeler I just followed the LDED workshop instruction attached to the plug-in (and only used different values). You should be able to find it in the content downloaded along with plug-in. Search for .docx file in LDED folder. It describes all the steps required to set LDED process simulation in AM Modeler so you should be able to recreate such analysis easily.

When you write input file or submit the job in CAE the software gathers all settings from the whole model (including AM Modeler) and saves them as keywords in the generated input file ready for analysis.

 

[Matthew_19]

Hi FEAWAY,

The attached file will be absolutely brilliant for helping me understand the project as I now know that the job will run for atleast three layers. I shall try follow the guide for LDED and locate the doc.x file to aid the understanding. I am not fully aware on how to select the top component as what needs built in the .CAE. - what i mean is how to select that one part is the substrate, the base plate, and the next part needs 'build up' in the .cae. Is it straight forward and the LDED explains this? Thank you so very much for compiling the job into an .inp which I can hopefully run in ABAQUS. Is there a way to run this job as an .inp and look at it through .CAE format? To see the necessary steps involved?


You have massively helped, thank you very much. From what I understand from reading the file, you managed to set out the deposition path and do an 'element activation' for the required elements inside the flux, is this true? Is this an element activation technique that gets build during the domain.. or is it more a birth & death technique where all elements are killed to start with then build as the domain grows?

Much appreciated FEAWAY!

 

[FEA way]

In the AM plug-in you can select which part is to be built using AM Parts option (click it with right mouse button and select Assign). But be careful when defining cooling - by default it will be applied only to the build part.

Yes, you can use File --> Import --> Model and switch to .inp files. This way the input file will be converted into CAE model. However not all keywords can be processed this way - some are not supported by Abaqus/CAE.

The progressive element activation technique used by Abaqus works in such manner that at the beginning of the simulation elements are inactive and then they are activated when material is deposited in their locations. Both full and partial element activation is available.

 

[Matthew_19]

Hi FEAWAY,

I have tried to view the results by running it through the .cae, however, many errors have raised during the job analysis:
Density has been defined as a function of temperature and/or field variables. For all elements except acoustic, heat transfer, coupled temperature-displacement and coupled thermal-electrical elements the density is a function of the initial values of temperature and field variables. It will not be updated if temperatures and field variables change during the analysis.

**Output request eactive is only available for elements with progressive activation**

**There is zero HEAT FLUX everywhere in the model based on the default criterion. please check the value of the average HEAT FLUX during the current iteration to verify that the HEAT FLUX is small enough to be treated as zero. if not, please use the solution controls to reset the criterion for zero HEAT FLUX.**

I think these problems may be due to trying to view the results in ABAQUS/CAE, how else can i see the results?

 

[FEA way]

I suggest the following approach:

- import the input file to CAE only if you want to view the settings. In order to run the analysis from CAE you will probably have to make some changes in the model (due to previously mentioned incompatibility of several keywords with CAE).

- if you want to run this job as it is and see the results then submit it from the input file using command window (e.g. abaqus job=input_file_name interactive)

 

[Matthew_19]

Hi FEAWAY, further to your post yesterday, I cannot locate any .docx file in the downloaded content. The only files that were available to be had the folder headings:

AMModeler - WHICH CONTAINS ALL PYTHON SCRIPTS FOR THE TABLES
AM_LECTURES_2017 - which only contained pdf documents (unsure - maybe it was this file you meant to follow? or do you mean the abaqus SIMULIA USER assisstance?

Or unless I need to donwnload something else also?

The file link I have is:

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

then click the download ABAQUS/CAE plugin on right hand side

 

[Matthew_19]

I have tried to run simulation via command prompt, these error messages failed the job:

***ERROR: Toolpath-mesh intersection module: Toolpath-Mesh intersection module
is not available.
Does this mean I cannot see the results? Or need to download something else

I am not sure how you managed to get the file to run, very strange!

 

[Matthew_19]

Very frustrating, no analysis will run due to this error message:


***ERROR: Toolpath-mesh intersection module: Toolpath-Mesh intersection module
is not available.
Even though I have ABAQUS plug in downloaded and installed

 

[FEA way]

Maybe this document is not provided for download anymore. It was included in plug-in content a few months ago but it’s possible that DS changed this content.

I used Abaqus 2019 to prepare this model and it works in this version. Apparently, some of the currently built-in AM utilities (including toolpath-mesh intersection module) in previous versions (including 2018) were only available in form of subroutines attached to the plug-in. Thus you will need respective AM plug-in version for Abaqus 2018. I’m not sure if it’s still available.

 

[Matthew_19]

Simulation won't run for me due to the above error, also where did you acquire these values:

*PARAMETER TABLE TYPE, NAME="ABQ_AM.MovingHeatSource.Goldak", parameters=10
INTEGER, , "SubDivX" , , ,
INTEGER, , "SubDivY" , , ,
INTEGER, , "SubDivZ" , , ,

being 9, 9, 9? I wasn't sure where you achieved these values

 

[Matthew_19]

Due to the plug in not being available, does this mean that non of the analysis will work? In my abaqus 2018? Which means I will have to resort to time dependent coordinates? With a Fortran Subroutine?

 

[Matthew_19]

When I downloaded the link, it was Abaqus2018 plug in so I am unsure why it's not working, the feature toolpath-mesh intersection doesn't work annoyingly. Any ideas how to get around this?

 

[FEA way]

Those three parameters (SubDiv X, Y and Z) represent the number of subdivisions along each of the local directions. I just used the value from workshop example.

It only means that you probably won’t be able to run the analysis from the input file that I prepared in newer version. But since you have plug-in for Abaqus 2018 and AM Modeler works properly when you use it in CAE then you should be able to set up the analysis following some examples. To learn how to use AM Modeler interface, check the lectures (pdf files) provided with the plug-in. To adjust the settings for your specific case you can examine the input file that I attached previously (open it in text editor).

If you fail to set everything up in AM Modeler, I will try to guide you by giving instructions of what should be done step by step (like in the workshop document). But it would be better for you to figure it out without such detailed guidelines because you should understand how these functionalities actually work to use them properly.