Get a points x , y value in existing sketch
Hello,
I am not sure if I get your point or not. Please refer to the following sample how to find non-driven dimension and associated points.
BTW: the codes are assuming there is a sketch in current design and there are two points and one non-driven dimension in the sketch.
Thanks,
Marshal
import adsk.core, adsk.fusion, traceback
import os
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
design = adsk.fusion.Design.cast(app.activeProduct)
root = design.rootComponent
sketch = root.sketches.item(0)
dimension = adsk.fusion.SketchLinearDimension.cast(sketch.sketchDimensions.item(0))
p1 = dimension.entityOne
p2 = dimension.entityTwo
ui.messageBox('Driven Dimension: {}, entity one: {}, entity two: {}'.format(dimension.isDriving, p1.objectType, p2.objectType))
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
Marshal Tu
Fusion Developer
>
The code below show part of what you need. It asks for a point selection and then reports it's location. Coordinates for sketch geometry will be returned with respect to the sketch coordinate system. If you want to find it's location in the model you can use the worldGeometry property instead of geometry. The hardest part of your request is finding that particular point. There will be a lot of sketch points in that sketch and you'll need to find something unique about that specific point. Possibly the type of constraints used to position it or maybe it's position relative to the other points. It would also be possible to add an attribute to the point, effectively naming it, so that you can find it again later. Without knowing your complete workflow it's difficult tp be very specific about a solution.
import adsk.core, adsk.fusion, traceback
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
pntSel = ui.selectEntity('Select a sketch point', 'SketchPoints')
if pntSel:
pnt = adsk.fusion.SketchPoint.cast(pntSel.entity)
ui.messageBox('Point: ' + str(str(pnt.geometry.asArray())))
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
If this is a ParametricDesignType, driven sketch dimensions will still have a parameter that will hold the value. In this case you could obtain the value with:
dim.parameter.value
But if the design is a DirectDesignType (non parametric), then the dimension will not have a parameter value. In this case, we do not have a convenience method to get the parameter value (normally it is obtained from the parameter). We should add a convenience method to get the dimension value and text directly from the dimension object (instead of going through the parameter). I will file an issue for this. But in the meantime, as you mentioned you can calculate it from the entities of the linear dimension. I believe they will always be sketch points, and in your case they definitely should be, so you could use code like the following to get the linear dimension's distance value.
dim = SketchLinearDimension.cast(ui.activeSelections.item(0).entity)
pt1 = SketchPoint.cast(dim.entityOne).geometry
pt2 = SketchPoint.cast(dim.entityTwo).geometry
dist = {
DimensionOrientations.AlignedDimensionOrientation: lambda: pt1.distanceTo(pt2),
DimensionOrientations.HorizontalDimensionOrientation: lambda: abs(pt1.x - pt2.x),
DimensionOrientations.VerticalDimensionOrientation: lambda: abs(pt1.y - pt2.y)
}[dim.orientation]()
ui.messageBox(str(dist))
Kris
Kris Kaplan
Hi Kris,
Thank you, I've been trying down this route, code below, but it only returns the named parameters.
def writeTheParameters():
app = adsk.core.Application.get()
design = app.activeProduct
result = ""
for _param in design.allParameters:
try:
paramUnit = _param.unit
except:
paramUnit = ""
result = result + "\"" + _param.name + "\",\"" + paramUnit + "\",\"" + _param.expression + "\",\"" + _param.comment + "\"\n"
print (result) Return Value
>>> d1","mm","35.00 mm",""
"d2","mm","75.00 mm",""
"d4","mm","50 mm",""
"d6","mm","20 mm","
>>>
My example sketch and parameters:
So I don't follow why the yellow highlighted driven dimensions are not printed?
Clearly they must be somewhere, probably d3 and d5 which appear to be skipped in the Model Parameter list. But how to access?
Thanks
In the GUI, the feature has been added in the Ver2.0.12157 update, so I tried it out in the API.
I have prepared a sketch like this.
Then, I created the script.
# Fusion360API Python script
import traceback
import adsk.fusion
import adsk.core
def run(context):
ui = adsk.core.UserInterface.cast(None)
try:
app: adsk.core.Application = adsk.core.Application.get()
ui = app.userInterface
des: adsk.fusion.Design = app.activeProduct
root: adsk.fusion.Component = des.rootComponent
skt: adsk.fusion.Sketch = root.sketches[0]
dims = skt.sketchDimensions
dims[1].parameter.expression = 'd1'
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
When I ran the script while I was in the sketching process, it worked fine, but when I ran it while I was out of the sketching process, I got an error.
It seems like a bug, but I couldn't quite figure out why.
