Abaqus Python scripting issue

[vhr]

Hello everyone,

I am currently trying to do a simulation using python scripts. I am modeling heat flow through pipe thickness but I am having a hard time defining a surface to which I want to apply constant temperature BC. I am attempting to apply Temp BC to the pipe surface but am not able to capture the surface I think. I am using the following script. I am getting an error message 'Set must contain some entities' at the last line in the script below. I am new to this so any help would be highly appreciated. Thanks in advance!

internal radius of the pipe = 0.1
length of the pipe = 1.0

internalPipePoint = (0.1, 0.0, 0.5)
internalPipe = myInstance.faces.findAt((internalPipePoint,))
intDiaRegion = regionToolset.Region(side1Faces=internalPipe)
myModel.TemperatureBC(name='Temp Int',createStepName='temp', region=intDiaRegion, magnitude=100.0)

Also, when trying to print 'internalPipe' and 'intDiaRegion' in the abaqus I am getting this output.

internalPipe: (mdb.models['Pipe'].rootAssembly.instances['pipeInstance'].faces.findAt(((0.1, 0.0, 0.5),)))
intDiaRegion: (Region(side1Faces=mdb.models['Pipe'].rootAssembly.instances['pipeInstance'].faces.findAt(((0.099154, 0.012978, 0.666667),),)))

 

[Mustaine3]

Maybe the face is not at the location you are searching. Create a datum point with those coordinates and see where it is.

You can also try getClosest().

 

[vhr]

Hi Mustaine3,

Thank you for your answer. I did create a datum point to check whether the specified point is there or not and it does seem onto the surface. I have attached the pipe images herewith for reference. And I have also used getClosest as below but it still shows the same error when ran, i.e, 'Set must contain some entities'.

internalPipePoint = (0.1, 0.0, 0.5)
#internalPipe = myPart.faces.getByBoundingCylinder((0.0,0.0,0.1),(0.0,0.0,0.9),0.12)
#internalPipe = myPart.faces.getByBoundingBox(0.0,0.0,0.1,0.1,0.1,0.9)
internalPipe = myPart.faces.getClosest(coordinates=((0.1, 0.0, 0.5),))
face_i = internalPipe[0][0].index
side1Faces = myPart.faces[face_i:face_i+1]

intDiaRegion = regionToolset.Region(side1Faces=side1Faces)
myModel.TemperatureBC(name='Temp Int',createStepName='temp', region=intDiaRegion, magnitude=100.0)

When printing 'internalPipe' and 'intDiaRegion', it gives following output in Abaqus now. I also tried using 'getByBoundingCylinder' and 'getByBoundingBox' but still the same error.

internalPipe: ({0: (mdb.models['Pipe'].parts['Part Pipe'].faces.findAt((0.1, 0.0, 0.5), (-1.0, 0.0, 0.0)), (0.1, 0.0, 0.5))})
intDiaRegion: (Region(side1Faces=mdb.models['Pipe'].parts['Part Pipe'].faces.findAt(((0.099154, 0.012978, 0.666667),),)))

 

[Mustaine3]

Upload the cae file and the script and I will have a look at it.

 

[vhr]

Hi Mustaine3,

I have uploaded the cae file and the script herewith. Please find it in the link below.

Link

 

[Mustaine3]

Loads, boundary conditions, contact, etc. are applied at the instance(s), so you have to use them instead the part to get the geometric entities. Or you generate a set/surface at part level and use the derived set/surface from an instance for those definitions.

Apply the load in the UI and look what the .rpy is reporting. If you don't get a .rpy because of the Student edition, then you might check if you can record a macro and look into that.

 

[vhr]

Hi Mustaine3,

I did initially apply BCs at Instance only but I changed it a day before sharing it with you to the 'Part' as I read on some other forum that it might solve the problem. But great advice there. I applied loads and BCs in the UI and checked out the file later. And it created Set before applying BC to it. I did the same and it worked for me along with 'getByBoundingCylinder'. Here's the final script. Thanks a lot.

innerPipeRadius = 0.1
outerPipeRadius = 0.15
pipeLength = 1.0

internalPipe = myInstance.faces.getByBoundingCylinder((0.0,0.0,-0.1),(0.0,0.0,1.1),0.12)
intDiaRegion = myAssembly.Set(faces=internalPipe, name='IntDia Set')
myModel.TemperatureBC(name='Temp Int',createStepName='temp', region=intDiaRegion, magnitude=1.0)