AM Modeler Plugin

[ZohrehA]

Hi,
I would like to model cold spray process (a coating process but also use for additive manufacturing) with AM modeler.

I am new at AM Modeler plugin, till now I was successful to create an event series for heat source.

But for adding material I have problem from the beginning. I found that I have to use Progressive Element Activation but I don’t know where or in which module I can define it? I either don’t know if I need subroutine for defining material addition or not?

In this stage I am not going to consider material property changes with temperature.

My model is a simple model: a flat rectangle part, with the initial room temperature. The maximum temperature that part reach during the process is about 300 ̊C (below melting point).
The heat source is a high pressure, high temperature Ni gas (P= 30 bar, T= 500 ̊C) that carries high velocity particle (about 800 to 1200 mm/s) through a de Laval nozzle. The nozzle travel above the surface and spray the high velocity high temperature particles on the surface. So the particles attach to the surface by their kinetic and thermal energy. The convection and radiation is considered. And only elastic property is define for material.

I have studied a lot of documents and ABAQUS documentation, but it is not clear for me that what is the first step and where and how I can define the Progressive Element Activation

Is anyone here that could help me in this regard?

 

[FEA way]

Progressive element activation is enabled using Material Input in AM Modeler. There you can specify all the settings of element activation (such as selecting partial/full activation).

 

[ZohrehA]

Thanks for your reply. You mean Material Arrival?

 

[FEA way]

In older versions, it was called Material Arrival and it used settings from proper table collection. In new versions, it’s called Material Input and settings are available directly there.

 

[ZohrehA]

Dear FEA way,
Thanks for your answer. It helped me. Just I have problem about defining some parameters.
I don't know what they mean?

One is "Activation offset" (in ABQ-AM.MaterialDeposition.Bead)?

And others are in "ABQ-AM.MovingHeatSource.Uniform". I don't know what are "SubDivx,y,z" ; "offset1,2,3" ; "BoxLength" and "absorption coef."?
Would you please give me a description?

My Heat Source is Hot Particles and Gas that are sprayed from a De Laval Nozzle. I am not sure if Uniform heat source is a good one or not? It is not a laser process, it is a coating process called cold spraying.

 

[FEA way]

AM process modeling functionalities are currently built into Abaqus and thus they are described in the documentation (Analysis Techniques --> Additive Manufacturing Process Simulation --> Special-Purpose Techniques for Additive Manufacturing).

The Activation offset parameter is not used and should be set to zero. The SubDiv, Offset and BoxLength parameters describe the box toolpath-mesh intersection. The absorption coefficient is a material property used for laser heating.

A uniform heat source is recommended for cases in which element size is comparable to laser spot size.

 

[ZohrehA]

Your answers were so helpful. I got the answer of most questions. Thank you so much.
Just:
1- I am not sure about the absorption coefficient. It is only for laser process?

My process is not a laser process. It is a kind of thermal spray process, that the heating source is hot N2 gas (500 to 1000 C) that heat up particles inside a nozzle + that high temperature, high velocity particles. Particles and substrate are Al and Ti.

Do you think in this case is it OK to put the absorption coefficient equal to 1??
Is this coefficient the same as emissivity?!

2-About the type of heat source: The exit diameter of the nozzle (as a heat source) is about 4-5 mm (the area that high temperature particles are carried by hot gas and deposited) and my mesh size is 1 mm. So do you think uniform heat source is suitable for this process? Or Goldak?!

 

[FEA way]

The absorption coefficient is relevant only for laser heating. On the other hand, the Goldak heat source is meant primarily for welding. In fact, your case of cold spray additive manufacturing is quite specific. Maybe you could try modeling it in a similar way as it’s done with the FDM process.

 

[ZohrehA]

Thanks a lot for your support.
I followed your advices. Done the same as FDM additive manufacturing. Now the material addition is working pretty good.

I used a uniform heat source. The parameters are as bellow:

"ABQ_AM_AbsorptionCoeff" = 1
"ABQ_AM_EnclosueAmbientTemp"= 32
"SubDivx,y,z"= 3
"offset1"= 0
"offset2"= 0.001 m
"offset3"= 0.000085 m (half of "BoxLength3" )
"BoxLength1" = 0.002 (equal to width of the Bead)
"BoxLength2" = 0.002
"BoxLength3" = 0.00017 (equal to thickness of the Bead)

The magnitude of Power in "ABQ_AM_PowerMagnitude" Event Series = 14500000 (J/s.m3, heat Flux)

Assign the Heat Source in Heating section of AM Simulation setup. Region --> use assigned build parts (select coating part)

Define Convection and Radiation in Cooling Section of AM Simulation setup.


Also in the Heat Transfer Model I defined the same convection and Radiation and Ambient Temperature in Interaction Module.

Defined body heat flux in Load Module, Distribution --> Uniform, Magnitude --> 14500000 J/s.m3

The Initial Temperature of Coating = 300 C and Substrate= 32 is defined at Predefined Field.

Although all above when I run the Model the temperature of the coating and substrate are very low (attached file). Substrate changes from 32 to 33 C, and Coating (with initial temperature of 300 C) goes to Max. 45 degree C.
I am wondering why the temperature is not changes?!!

Would you please help me if you have any idea about this problem?
Thank you in advance.

 

[FEA way]

It's often a fault of too low power - double-check its unit and value. Also, try to visualize the box representing the heat source and see how it intersects with mesh.

 

[ZohrehA]

I have used this amount of Heat flux in a simple model (not AM), and I get the Max. Temperature of about 250 C.
So I don't think so it is a low Heat Flux.
It is Strang that temperature of coating will be decrease to 48 C from 300 C !! I set the initial temperature of coating equal to 300 C.

What do you mean by "intersect the box with mesh".
If you mean the moving path I have checked the event series toolpath of heat source, in my opinion it is OK .

 

[FEA way]

I’ve just noticed that you defined convection/radiation and body heat flux manually. This is not necessary, the plug-in will define cooling and heating based on the settings of the AM Model. Remove those duplicated manual definitions and see if it works as expected then. Leave only initial conditions and boundary conditions (if there are any) in the Model tab.

 

[ZohrehA]

Dear FEA way,
Thanks for your guide. Ok I will try your point and delete convection and radiation interaction in static model and only define them in AM plug in cooling and heating section. Just how should I define a temperature dependent heat transfer coefficient (h) for convection in AM Plug in?

 

[FEA way]

It can't be done directly in the plug-in but you can create a film property in the Model tab and then, after finishing the setup in the plug-in and exporting the input file, replace the last value in the *FILM keyword's data line with the name of the film property created before.

 

[ZohrehA]

You mean first I have to create and complete the model in AM Plugin with a single number for heat transfer coefficient in convection -->Cooling simulation part of the AM Plugin. Then close the ABAQUS CAE and go to the working directory and open the .inp file and there find the *FILM data line and replace the number with the name that I have created in film property?

As you said in 2 comment ago, I have to delete convection/radiation and body heat flux in normal Model tree and only define them in AM Plugin, yes? So in this case should I only define a file property in Model tree without defining convection and then use it later in .inp file? Does it transfer to AM Model and work properly?

 

[FEA way]

Yes, you should do exactly what you described. Ultimately, it all comes down to keywords - as long as they are correct, the analysis will run properly.

 

[ZohrehA]

Thank you so much.
I have done the same as you said.
First I did 'write input' in Job Manager, then I opened created .inp file and changed the *FILM data there, then I submited the job and ran it. But after running when I opened the .inp file again I saw that the *FILM is changed to the number (the same as Cooling in AM plugin)!!

Also the temperature didn't go up as well, though I have defined the convection, radiation and heat flux only in AM plugin (and deleted them in normal thermal model)!

Could I send you the .cae file (ABAQUS 2022) to check it if it is possible.
I really cannot find out what is the problem?

 

[FEA way]

Did you import the .inp file to Abaqus/CAE after editing it ?

 

[ZohrehA]

Import?! How?

 

[FEA way]

After editing the input file you should submit the analysis directly from the command line, without opening this input file in Abaqus/CAE and submitting from it.