Automation and iteration in Workbench

M

A customer had a request to make the number of design parameter sets dependent on the result of a solution. So I put together a few lines to do exactly that.

The script below can be run in Workbench.

It will iterate on the parameterized load (a simple force) until the given deflection parameter is reached. (as a control, a max ctr was also used).

So it starts, runs one analysis, then checks if the deflection criteria is met and if not goes into a loop to increase the force load by 10% until the criteria is satisfied.

Example Script:

Reset()

""" This script will create an iterative DP Ansys run"""

import tempfile, os
tempdirectory = tempfile.gettempdir()

name = "myTest.wbpj"

saveName = os.path.join(tempdirectory,name)
import time

t1 = time.time()

X = 1000

Y = 1000

Z = 1000

Load  = 1000

fx = 'fixFace'

lx = 'loadFace'
Some iteration parameters
maxDef = 7E-06 # goal to cut out

deltaForcePercent = 1.1 # value to multiply myInput

maxctr = 10 # control for to avoid looping too long
cmd = """

P0 = Point.Create(MM(0),MM(0),MM(0))

P1 = Point.Create(MM(%s),MM(%s),MM(%s))

BlockBody.Create(P0,P1)

"""%(X,Y,Z)
myTemplate = GetTemplate(TemplateName="Static Structural",Solver="ANSYS")

mySystem = myTemplate.CreateSystem()
geometry = mySystem.GetContainer(ComponentName="Geometry")

geometry.Edit(IsDiscoveryGeometry = True, Interactive = True)

geometry.SendCommand(Language="Python", Command=cmd)

geometry.Exit()
modelContainer = mySystem.GetContainer(ComponentName="Model")

modelComponent = mySystem.GetComponent(Name="Model")

modelComponent.Update(AllDependencies=True)
mechcmd = """

ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardNMM
Mesh
M = ExtAPI.DataModel.Project.Model.Mesh

M.ElementSize = Quantity('500 [mm]')

M.CreateParameter('ElementSize')
Fixed Support
NS = Model.AddNamedSelection()

NS.ScopingMethod=GeometryDefineByType.Worksheet

NS.Name = "%s"

Criteria = NS.GenerationCriteria

Criteria.Add(None)

Criteria[0].EntityType = SelectionType.GeoFace

Criteria[0].Criterion = SelectionCriterionType.LocationY

Criteria[0].Operator = SelectionOperatorType.Equal

Criteria[0].Value = Quantity('0 [mm]')

NS.Generate()
NS = Model.AddNamedSelection()

NS.ScopingMethod=GeometryDefineByType.Worksheet

NS.Name = "%s"

Criteria = NS.GenerationCriteria

Criteria.Add(None)

Criteria[0].EntityType = SelectionType.GeoFace

Criteria[0].Criterion = SelectionCriterionType.LocationY

Criteria[0].Operator = SelectionOperatorType.Equal

Criteria[0].Value = Quantity(str(%s) + ' [mm]')

NS.Generate()

F= Model.Analyses[0].AddForce()

F.Location = ExtAPI.DataModel.GetObjectsByName("%s")[0]

F.DefineBy = LoadDefineBy.Components

F.YComponent.Output.SetDiscreteValue(0, Quantity(%s, "N"))

F.CreateParameter('ComponentY')
B = Model.Analyses[0].AddFixedSupport()

B.Location = ExtAPI.DataModel.GetObjectsByName("%s")[0]
Add Result Total Deformation
TD = ExtAPI.DataModel.Project.Model.Analyses[0].Solution.AddTotalDeformation()

TD.CreateParameter('Maximum')

"""%(fx,lx,Y,lx,Load,fx)
modelContainer.SendCommand(Language="Python", Command=mechcmd)

modelContainer.Edit(Interactive=False)

t2 = time.time()
designPoint1 = Parameters.GetDesignPoint(Name="0")

parameter1 = Parameters.GetParameter(Name="P1")

parameter2 = Parameters.GetParameter(Name="P2")
Save(FilePath = saveName,    Overwrite=True)
print('time = ' + str(round(t2-t1,2)))
iteration loop
##dp1 = Parameters.GetDesignPoint(Name="0")

myInputParameter = Parameters.GetParameter(Name="P2")#

myInputValue = myInputParameter.Value.Value

inputUnits = myInputParameter.Value.Unit
newInputValue =  deltaForcePercent*myInputValue

backgroundSession1 = UpdateAllDesignPoints(DesignPoints=[designPoint1])

myOutput = Parameters.GetParameter(Name="P3").Value.Value
ctr = 0

while myOutput <= maxDef and ctr <= maxctr:

print('Deflection goal not reached, will iterate')

dpX = designPoint1.Duplicate()

Parameters.SetBaseDesignPoint(DesignPoint=dpX)

newInputQuantity = str(newInputValue) + ' [' + inputUnits+']'

print(newInputValue)

dpX.SetParameterExpression(Parameter=myInputParameter,Expression = newInputQuantity)

backgroundSession1 = UpdateAllDesignPoints(DesignPoints=[dpX])

myOutput = Parameters.GetParameter(Name="P3").Value.Value

newInputValue =  deltaForcePercent*myInputParameter.Value.Value

print('New Force Load = ' + str(newInputValue))

ctr+=1

Parameters.SetBaseDesignPoint(DesignPoint=designPoint1)

Mike.Thompson

While I can see the value in this implementation I want to offer some other parallel suggestions for similar use cases:

1. You can do this same script concept in Mechanical alone without the need of parameters. You could simply solve>update force value in a loop until criteria is met. The benefit of this is less overhead of opening/closing Mechanical like the design points do on each iteration. The code would likely be even smaller as well. The problem is you don't have all the design points data unless you store them yourself.
2. The other option is to use built in WB design optimization. This would be especially helpful if the output criteria and inputs are more complex. Optimization routines will try to get to the desired criteria as efficiently as possible by creating/reading 'response surfaces' and doing multi-dimensional interpolation to converge on desired values. This can be done with built in components without scripting.

M

@Mike.Thompson I agree.

The original customer query wanted to stay in Workbench and update geometry which likely means going back to Disco/Spaceclaim (and opening/updating). The example was designed to show how a WB output parameter (here from Mechanical) could be used to determine if a new DP was required.

And I, like the customer, see python as the hammer and all challenges as nails.

Mike.Thompson

Perhaps this post would also be of interest in this case of modifying geometry.

https://discuss.ansys.com/discussion/2422/example-how-to-use-different-geometry-files-parametrically-in-workbench-mechanical