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

 

[Matthew_19]

Okay I shall try to understand the functionalities in the AM modeller. The only problem I have is defining the toolpath intersection, in the respect that it doesn't work on my ABAQUS 2018, but surely there must be another way like you've suggested. I will try to work this out and see if it works using the prior examples.

 

[Matthew_19]

Hi FEAWAY,

I have now downloaded the ABAQUS19 version, does this still mean I would a FORTRAN SUBROUTINE written for the heat source model and such or does the AM modeller build all the subroutines needed? Do I need a compiler built into the computer also?

 

[FEA way]

Abaqus 2019 has all the necessary features built-in. There’s no need to define any subroutines. Thus you should be able to run the analysis from the input file that I shared here previously. And you can configure your own simulation either using plug-in (which now serves as automatic keyword generator) or manually editing input file.

 

[Matthew_19]

Would you be able to send the doc.x file across for the AM plug in that contains the workshop LDED? It means I could work my way through the example just changing values?

 

[FEA way]

I downloaded the plug-in again to check what changed in the content attached to it. As you said, the docx document is not there but in readme.txt file they say that workshop resources were moved to Knowledge Base. Thus you can find all the files (including those related to LDED example that you are looking for) if you visit Dassault Systemes Knowledge Base, log in to your 3ds account and search for QA00000057533 (article titled "Abaqus/CAE Plug-in Utility for Additive Manufacturing Process Simulation"). From there you can download not only the document with description of LDED workshop but also all necessary model files (cae, jnl, inp).

 

[Matthew_19]

Thanks very much FEAWAY, I have proceeded with this route. Further to the analysis that you carried out, did you notice that not all the elements were built and there was some elements missing throughout the build?

 

[FEA way]

Yes, the issue is most likely about matching toolpath and mesh density or adjusting "ABQ_AM.MaterialDeposition.Bead" settings.

 

[Matthew_19]

Thanks FEAWAY. I was further wondering, when the heat source is applied to the top part needing built and as it's getting built. Did you notice the base plate conducting heat? Couldn't notice it in the .inp file you sent across, infact, couldn't see the base plate at all. Is this a problem with set up?

 

[FEA way]

The cae file that you’ve attached here contains only a single part and its assembly instance. So I assumed that this is the build part and that the base plate can be ignored. In such analyses it’s not always necessary to include the base plate.

 

[Matthew_19]

Apologies, the part I am working with contains two parts:

a base plate made from IN718 and going to deposit IN718 on top of the base plate.

Part-1 was the base plate and Part-2 was the deposit structure.

Is there a way to carry out analysis as usual but further include the base plate as heat is conducted through such part with clamping fixtures? So the temperature from heat source, melt pool and deposition effects not only the built part but the base plate?

Only part-2 is to be build but part-1 is to experience transient temperature field also? Is this possible to include in analysis?

 

[Matthew_19]

The assembly instance was to show where the deposit would occur on the base plate, is this not how you would show?

 

[FEA way]

Sure, base plate can be added to the analysis so that its participation in heat transfer is included. Just make sure that the part to be built is selected in AM Parts option of the AM plug-in and (as I’ve mentioned in one of the previous posts) keep in mind that by default the base plate won’t be cooled. You have to add it to the cooling definitions manually.

Build part must have its final geometry modeled and meshed just like the base plate. That’s because even though the build part elements seem to appear during the analysis, they must exist in the model (in inactive form) from the beginning of the simulation.

 

[Matthew_19]

I understand this now FEAWAY, makes sense. Would you define the base plate cooling conditions in the CAE as a separate step? Or would you just add it to the cooling section on the tree as a part? If this makes sense..

The final geometry of both the build part and base plate makes sense, as the elements within the build part activate during deposition. I just want to show that the build part experiences not only heat conduction but cools as with the build part, but at the start of the analysis, the base plate is fully activated.. if this makes sense?

 

[FEA way]

The easiest way to add cooling for base plate is to replace build part ELSET in *FILM and *RADIATE keywords with ELSET containing all elements in the model (base plate and build part elements). AM parts are cooled with the use of progressive cooling. This feature applies convection and radiation only to the surfaces exposed to environment. So when new layer of elements becomes active, the previous one stops being cooled at the surfaces covered by new layer.

 

[Matthew_19]

Thank you very much FEAWAY, this makes sense. As they are continual elements, I take it they keep cooling until ambient temperature depending on step time also?

 

[FEA way]

If you want to simulate the whole cooling process you should define large enough analysis step time (extending far beyond the last moment of heating). To determine the time required for the model to reach steady state you should monitor temperature variations at global level (using contour plots) and at selected points (using xy data from history or field output).

 

[Matthew_19]

This is excellent advice, I am currently in the process of building the simulation in both ways - currently using DFLUX FORTRAN subroutine and the AM plug. Thank you very much for the help FEAWAY. I shall apply a step time far surpassed the required heating time - this is a good point.

 

[Matthew_19]

Hi FEAWAY,

See if I want the Heat to directly effect the build part and base plate, like I asked for cooling.. Would this be done in the same way as in the AM model plug in:
-Heating > create> under region 'use element set (picked)' and select the element set that includes your whole model, including the build part and base plate? If this makes sense.

Cheers

 

[Matthew_19]

Furthermore, What element types did you use? I used DCC3D8 and it does not comply with MBFNU function? Would this be correct? I thought it would be heat transfer elements

 

[FEA way]

In the AM plug-in (under Heating) you only define heating via the moving heat source (laser). If you want to apply some additional thermal boundary conditions to the base plate, you should do this in the Model tree (outside of the plug-in). Or add necessary keywords to the input file.

I used DC3D8 elements for this analysis. They are regular heat transfer elements whereas DCC3D8 means convection/diffusion elements.