How can I automatically setup the imported load data from Maxwell inside mechanical thermal analysis

Below is a mechanical script, that reads the time steps from a Maxwell file (AnsoftTransferData.xml), creates an imported load (heat gen.), and then adds all of the rows + corresponding input data (source and analysis times - taken from the Maxwell file).

model = ExtAPI.DataModel.Project.Model
Parts = model.Geometry.GetChildren(DataModelObjectCategory.Part,True)
first_analysis = ExtAPI.DataModel.Project.Model.Analyses[0] 
solver_directory = first_analysis.WorkingDir
file = solver_directory+"Maxwell3DSolution\AnsoftTransferData.xml" # this folder might need change, so we should find the Ansoft xml file
 
SolveOutLines = [] #Declare an empty list
mytime=[]
myind=[]
with open(file, "r") as in_file:
    for line in in_file: #For each line of text store in a string variable named "SolveOutLines", and
        SolveOutLines.append(line)  #add that line to list of lines.
myind=SolveOutLines[0].split("<TIME>")
myind.pop(0)
for myt in myind:
    mytime.append(myt.split("</TIME>")[0])
 
impLoadGrp = ExtAPI.DataModel.GetObjectsByName('Imported Load (B4) ')[0] # change as needed
heatGen=impLoadGrp.AddImportedHeatGeneration()
selection = ExtAPI.SelectionManager.CreateSelectionInfo(SelectionTypeEnum.GeometryEntities)
bolist=[]
ids=[]
for Part in Parts:
    for Body in Part.Children:
        bolist.append(Body.GetGeoBody().Id)
selection.Ids=bolist
heatGen.Location = selection
 
for myrow in range(0,len(mytime)-1):
    table=heatGen.GetTableByName("") # get the worksheet table
    if float(mytime[myrow])>0.005: # change as needed - get times above 0.005 sec, to avoid initial small time steps
        NewRow = Ansys.ACT.Automation.Mechanical.WorksheetRow()
        table.Add(NewRow)
        NewRow[0]=mytime[myrow]
        NewRow[1]=mytime[myrow+1]
        NewRow[2]=mytime[myrow+1]
        NewRow[3]=1
 
table.RemoveAt(0)
ExtAPI.DataModel.Tree.Refresh()
heatGen.ImportLoad()