Script to change parameter values
It is fairly simple to edit the user parameters. Model parameters are also possible but a little more difficult because they can be scattered around in various components whereas there is only one set of user parameters for the entire design.
The program below changes two user parameters called "Length" and "Height" and depending on how you answer the message box will change them to one of two sets of values. You can change the names to whatever your parameters are called. Setting the expression property is exactly the same as changing it in the dialog and it supports all of the same things. For example you can specify the units as part of the string, i.e. "3 in" or "2 mm". Just "3" will default to 3 of whatever the current design unit is. You can also use equations and reference other parameters. For example, "(3 + Length)/2". If you use the "Scripts and Add-Ins" command to create a new script you can copy the code below and replace the run function in the created code. Then you can run it from the "Scripts and Add-Ins" command.
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
des = adsk.fusion.Design.cast(app.activeProduct)
userParams = des.userParameters
if ui.messageBox('Change to configuration one?', 'Parameter Edit', adsk.core.MessageBoxButtonTypes.YesNoButtonType, adsk.core.MessageBoxIconTypes.QuestionIconType) == adsk.core.DialogResults.DialogYes:
userParams.itemByName('Length').expression = '50'
userParams.itemByName('Height').expression = '30'
else:
userParams.itemByName('Length').expression = '30'
userParams.itemByName('Height').expression = '20'
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
I forgot about the Design.allParameters property. This returns all of the parameters in design, both Model and User parameters so using that makes it easy to use both.
Patrick Rainsberry
Developer Advocate, Fusion 360
Actually it is a reference to the actual body object. So you would do something like:
# Get application reference
app = adsk.core.Application.get()
design = app.activeProduct
#Get Root Component
rootComp = design.rootComponent
# Get All bodies in Design
bRepBodies_var = rootComp.bRepBodies
# Find the body with a given Name
body = bRepBodies_var.itemByName('My body Name')
# Set visibility of the Body
body.isVisible = True
Patrick Rainsberry
Developer Advocate, Fusion 360
You changed 'My Body Name" to the name of the body in the design, correct? Note it is case sensitive. The error means that it is not finding the body of that name.
You can check if an object is "None" in python with:
if body is None:
# OR:
if body is not None:So it would look something like this:
# Get application reference
app = adsk.core.Application.get()
design = app.activeProduct
#Get Root Component
rootComp = design.rootComponent
# Get All bodies in Design
bRepBodies_var = rootComp.bRepBodies
# Find the body with a given Name
body = bRepBodies_var.itemByName('My body Name')
# Set visibility of the Body
if body is not None:
body.isVisible = True
Patrick Rainsberry
Developer Advocate, Fusion 360
Oh also if the bodies you are looking for are not in the root COmponent and are in a sub component then you would need to call the brep bodies on the component you are interested in not the root component? Maybe this is the problem?
Patrick Rainsberry
Developer Advocate, Fusion 360
Ok here this should work. Kind of long for what you are trying to do but it looks like there is not an itemByName method on components:
#Author-
#Description-
import adsk.core, adsk.fusion, traceback
def run(context):
ui = None
try:
# Get application reference
app = adsk.core.Application.get()
design = app.activeProduct
# Get all components in design
allComponents_var = design.allComponents
# Loop through all components
for component_var in allComponents_var:
# Find the correct compoenent
if component_var.name == "My Component":
# Get All bodies in Component
bRepBodies_var = component_var.bRepBodies
# Find the body with a given Name
body = bRepBodies_var.itemByName('My Body')
# Set visibility of the Body
if body is not None:
body.isVisible = True
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
Patrick Rainsberry
Developer Advocate, Fusion 360
