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How to collinear constrain a line?

albie0803

albie0803

Alibre Super User
I define points and create a polyline starting at 0,0 and ending at 0,0, the first 2 points defining what becomes a vertical line from 0,0. How do I then use the constraint command to collinear constrain this line to the Y axis?
 
NateLiquidGravity

NateLiquidGravity

Alibre Super User
Hmmm, It seems PolylinePoints can not be used for constraints (according to the error "Exception: Only sketch figures can be passed to AddConstraint" and I'm not sure how to get line segments from the polyline. I also don't see a way to constrain directly to an axis or anything projected from 3d - yet.

My best suggestion is to create it as individual lines instead of polyline and then add the horizontal or vertical constraints directly to them.

Code: 
MyPart = Part('My Part')
MySketch = MyPart.AddSketch('SomeName', MyPart.XYPlane)

p1 = [0, 0]
p2 = [0, 10]
p3 = [10, 10]
p4 = [10, 5]

line1 = MySketch.AddLine(p1, p2, False)
line2 = MySketch.AddLine(p2, p3, False)
line3 = MySketch.AddLine(p3, p4, False)

MySketch.AddDimension(line1.Start, line1.End)
MySketch.AddDimension(line2.Start, line2.End)
MySketch.AddDimension(line3.Start, line3.End)

result = MySketch.AddConstraint([line1],Sketch.Constraints.Vertical)
print(result)
result = MySketch.AddConstraint([line2],Sketch.Constraints.Horizontal)
print(result)
result = MySketch.AddConstraint([line3],Sketch.Constraints.Vertical)
print(result)
 
albie0803

albie0803

Alibre Super User
@NateLiqGrav Thanks! I came to the same conclusion thinking about it last night in bed that I would have to use individual lines rather than a polyline for constraining. Being able to add constraints and dimensions will help immensely in scripts. At the moment scripted sketches are great unless you need to manually edit them.
 
albie0803

albie0803

Alibre Super User
I load variables into polyline points from an excel file. The file has 2 columns: diameter and length. I start by measuring a shaft and entering all the steps in it. I did one shaft that had 15 steps in it. The point being I will never have a set amount of variables.

From looking at the above discussion, I need to define lines to use dimension or constrain.

How do I define the name of a variable on the fly?

line1 = MySketch.AddLine(p1, p2, False)
line2 = MySketch.AddLine(p2, p3, False)
line3 = MySketch.AddLine(p3, p4, False)
etc
linex = MySketch.AddLine(py, pz, False)

or will I have to have twenty or so pre defined and have the code drop out when all values have been imported?
 
Last edited:
idslk

idslk

Alibre Super User
Hello colleagues,

isn't that valid in 2019?
NateLiqGrav said:
Some things to be cleared up:
  • Some functions do not have a return (void) so there is no need to assign it to a variable. For example AddCircle and AddPolygon have no return, that's why the console says "added Circle: None":
Click to expand...
if it is still valid, trying to assign a line to a variable won't be successful...
if it is overhauled in V2019 in some kind, try this:
Code: 
cp = CurrentPart()
mysketch = cp.AddSketch('MySketch', cp.XYPlane)

lines = []
p = [[10,13],[24,10],[18,26],[44,36]]
#Fill p with values from whereever, using some analogous like p.append(excelcells) or so

for i in range(0,len(p),2):
  print p[i]
  lines.append(mysketch.AddLine(p[i], p[i+1], False))

print lines
print 'done'

Regards
Stefan
 
ajayre

ajayre

Alibre Super User
Code: 
MyLines = []
MyLines.append(MySketch.AddLine(...))
for Line in MyLines:
  ...

Andy
 
NateLiquidGravity

NateLiquidGravity

Alibre Super User
Some things to be cleared up:
  • Some functions do not have a return (void) so there is no need to assign it to a variable. For example AddCircle and AddPolygon have no return, that's why the console says "added Circle: None":
Click to expand...
When I said this it was prior to having that ability in the 2019 beta. But the point I was trying to make still stands: We need to look at the reference to see what is expected to be returned (or if anything is at all).
 
albie0803

albie0803

Alibre Super User
@ajayre Can we get a list of constraint types that work please?

I want to be able to constrain a line end/start to the origin point. To anchor the sketch but still have it flexible (if that makes sense)

Profile.AddConstraint([Line.Start, Profile.Origin],Sketch.Constraints.Concentric)

Thanks to all for your input. Except for this last line I have the script now doing what I want. Now just have to wait for 2019 to be released.
 
ajayre

ajayre

Alibre Super User
NateLiqGrav said:
From my post in the Beta forum:

The (AlibreScript) documentation however does not list the options and only says:
Click to expand...

This is fixed for the next beta (or full release) of AD. But that's a documentation issue rather than what works or doesn't as you found out with the ordering of adding constraints.

Andy
 
albie0803

albie0803

Alibre Super User
NateLiqGrav said:
print(dir(Sketch.Constraints))
Click to expand...

['Coincident', 'Collinear', 'CompareTo', 'Coradial', 'Equal', 'Equals', 'Fix', 'Format', 'GetHashCode', 'GetName', 'GetNames', 'GetType', 'GetTypeCode', 'GetUnderlyingType', 'GetValues', 'HasFlag', 'Horizontal', 'Intersection', 'IsDefined', 'MemberwiseClone', 'Midpoint', 'Normal', 'Parallel', 'Parse', 'Perpendicular', 'ReferenceEquals', 'Symmetric', 'Tangent', 'ToBoolean', 'ToByte', 'ToChar', 'ToDateTime', 'ToDecimal', 'ToDouble', 'ToInt16', 'ToInt32', 'ToInt64', 'ToObject', 'ToSByte', 'ToSingle', 'ToString', 'ToType', 'ToUInt16', 'ToUInt32', 'ToUInt64', 'TryParse', 'Vertical', '__and__', '__class__', '__delattr__', '__doc__', '__eq__', '__format__', '__ge__', '__getattribute__', '__gt__', '__hash__', '__init__', '__invert__', '__le__', '__lt__', '__ne__', '__new__', '__nonzero__', '__or__', '__rand__', '__reduce__', '__reduce_ex__', '__repr__', '__ror__', '__rxor__', '__setattr__', '__sizeof__', '__str__', '__subclasshook__', '__xor__', 'value__']

So Concentric is not an option so

albie0803 said:
Profile.AddConstraint([Line.Start, Profile.Origin],Sketch.Constraints.Concentric)
Click to expand...

is not possible. I would have thought that being able to anchor a line end or circle centre to the origin would have been one of the first thing to be done. :confused: Oh well. :(
 
albie0803

albie0803

Alibre Super User
Why does this line

Code: 
Profile = P.AddSketch("Profile", P.GetPlane("XY-Plane"))
Profile.AddConstraint([Line, Profile.YAxis],Sketch.Constraints.Collinear)

throw the following error?

Code: 
AttributeError: 'Sketch' object has no attribute 'YAxis'
 
Last edited:
ajayre

ajayre

Alibre Super User
The axes don't really exist in sketches when looking at the AD API. What you want to do is not supported in the AD API as far as I can tell - submit a request to support.

Also if you want concentric constraints then submit a request to support... Andy
 
NateLiquidGravity

NateLiquidGravity

Alibre Super User
albie0803 said:
So Concentric is not an option so
Code: 
Profile.AddConstraint([Line.Start, Profile.Origin],Sketch.Constraints.Concentric)
is not possible. I would have thought that being able to anchor a line end or circle centre to the origin would have been one of the first thing to be done. :confused: Oh well. :(
Click to expand...
The new beta does list available options in the reference. No need to print that anymore.

Neither of those objects are circles or arcs. They are sketchpoints. Try Coincident instead.

Concentric is just a shortcut to make arcs and circles have the same center point. So internally it gets the centers and does a Coincident constraint with some makeup of a different icon.
 
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