How cn I do Natural Convection?

[Jay Prajapati]

In my model I'm doing plastic extrusion simulation with motion of nozzle simultaneously. So material is flowing continuously and when material comes out of nozzle I want to add convection and conduction.
1)I want to do natural convection with melted material with the air. so how can I do interference melted semi solid part.
2) How to do conduction between glass plate and melted solid?
so how to manage interference of this to surfaces?

 

[FEA way]

For conduction you will need thermal contact definition between extruded material and build plate. For convection you would have to apply film condition to appropriate faces of extruded material. To make it active only when material is already outside of the nozzle you would have to create a new step for cooldown.

Take a look at the „Extrusion of a cylindrical metal bar with frictional heat generation” in Example Problems Guide part of the documentation.

 

[Jay Prajapati]

thank you for response. I got your point but for conduction is it ok to make surface to surface interference between plate surface and whole extruded material? or better use nodes of extruded material instead of whole part?
2) in convection that is the problem that I have not clear body. I will apply convection in next step. so can you please elaborate which body part can I choose and how?

 

[FEA way]

Apply thermal contact interaction only to the part of extruded material which will likely touch the build plate. So mainly bottom and some side region. You will need mechanical contact between these parts anyway so you can use a single interaction for both mechanical and thermal contact. General contact can be used instead of surface to surface one.

For convection it will be similar. You have to predict which parts will be exposed to air. In this case you can assign film condition to bottom and both sides of the extruded material. Maybe even top region if the material is extruded completly.

 

[Jay Prajapati]

still for convection I'm confused that how to used. Cause the part coming is normally at room temperature and inside nozzle its conduction and the I want to give that extruded material a convection. so can I cut my part with datum plane and then choose only that part?

 

[FEA way]

Film condition for convection is applied only on the outer surface of the 3D body since convection occurs in the interface between this outer surface and surrounding air. Thus you just have to apply film condition to outer faces of extruded material which will be exposed to air after extrusion. It’s not a problem that they are initially inside the nozzle where convection does not occur. To account for this just create additional step for cooling and activate film condition in this step only, as I suggested before.

Of course you can use partitions if you don’t want to apply film condition to whole outer surface of the polymer part.

If you download one of the input files attached to the example from the documentation that I mentioned before and import this model to Abaqus you wil see how they did this.

 

[Jay Prajapati]

Hello Sir I got your point. but I have one more problem that after completion of my first step(Material comes down until glass) simulation stops. just start step 2 but it stops in 1 increment only can you just tell me how can I solve this error?

 

[FEA way]

Are there any errors reported in the Job Monitor (or msg/dat files if you run this job from command line) ? If there are no errors what are the warnings reported ? Abaqus must somehow indicate the reason why analysis suddenly stops.

 

[Jay Prajapati]

you can check here

 

[Jay Prajapati]

And here is data file

 

[FEA way]

The error you get („Too many attempts made for this increment”) indicates some convergence issues but with no details. From all the warnings the most alarming are these referring to negative eigenvalues. Remaining warnings indicate large distortion. Instead of coupled temp-displacement I would try dynamic tem-disp explicit analysis step. Your simulation involves very large deformations when polymer is extruded (that’s why in previous threads I was advising you to use other methods such as SPH or CEL). It will be hard to have convergence. But you will have much higher chances with explicit solver.

 

[Jay Prajapati]

In explicit I have problem with time. I gave total time 15 sec with 0.002 m/s velocity but its stops with the error that it needs more increment.

 

[FEA way]

Can you attach files generated from explicit analysis too ? And maybe a screen of job monitor.

 

[Jay Prajapati]

[URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1566830942/tips/Explicit_All_Part_upcy3w.dat[/url][URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1566830957/tips/All_Together_wgth1n.msg[/url]

 

[FEA way]

These warnings about inactive DOFs are nothing to worry about. In this case they mean that you applied boundary condition on DOFs 4,5,6. These are rotational degrees of freedom which for solid elements are not used.

Isn’t this .msg file the same as before (from implicit analysis) ? Could you check it and add a file from explicit simulation if I’m right ?

 

[Jay Prajapati]

[URL unfurl="true"]https://res.cloudinary.com/engineering-com/raw/upload/v1566900510/tips/Explicit_All_Part_bqh0g7.dat[/url]
In explicit is it possible to do simulation with big total time in step? like in one step 15 second?

 

[FEA way]

Yes, but unfortunately the longer event time the higher computational cost in terms of time required for the analysis to complete. That’s why it is even advised to artificially reduce the time of event in the simulation. It may alter results (sppeding up the analysis will increase the effect of inertia forces) but provides efficient way of reducing the analysis time significantly. Another way of lowering this computational cost is to use mass scaling.

The file attached is .dat file. It features warnings but no errors. Do you have .msg file for this simulation ?

 

[Jay Prajapati]

Is it possible with fine mesh to get result in standard(coupled-temperature-displacement)?

 

[FEA way]

Theoretically it may be possible but in practice it will be extremally hard because of the large deformations. Fine mesh won’t do much here.

The message file is empty. Apparently solver only generated the dat file. However it features no errors even though there are some in the monitor. Can you show the picture of the job monitor again but this time with Errors tab open ? Or attach input file for this analysis if you can.

 

[Jay Prajapati]

Ok here it is.