[bug] addByThreePoints method fails to create arc if the 3 points are too close

[JeromeBriot]

Hello,

The code below crashes whereas the 3 points are disctinct. Setting the factor value f to 100 solves the issue.

The error message:

RuntimeError: 5 : Some input argument is invalid.

It seems that there is a problem with the precision of the numbers during the computation.

import adsk.core, traceback

p1 = [-0.00047752000000000005, 0.15192502000000002]
p2 = [-0.0006226001152828134,  0.15214303759958947]
p3 = [-0.0006731,              0.1524]

# The code works with f = 100
f = 1

def run(context):

    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface

        product = app.activeProduct
        rootComp = product.rootComponent
        sketches = rootComp.sketches
        sketchesPlane = rootComp.xYConstructionPlane
        sketch = sketches.add(sketchesPlane)

        arcs = sketch.sketchCurves.sketchArcs

        pt1 = adsk.core.Point3D.create(p1[0]*f, p1[1]*f, 0.0)
        pt2 = adsk.core.Point3D.create(p2[0]*f, p2[1]*f, 0.0)
        pt3 = adsk.core.Point3D.create(p3[0]*f, p3[1]*f, 0.0)

        arcs.addByThreePoints(pt1, pt2, pt3)

        ui.messageBox('OK')

    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

The issue occurs when trying to import a geometry from a file.

Here are all the triplets values that failed:

*****
-0.00047752000000000005 0.15192502000000002 0.0
-0.0006226001152828134 0.15214303759958947 0.0
-0.0006731 0.1524 0.0
*****
0.21081746 4.1827069 0.0
0.21083651 4.182706638774926 0.0
0.21085556 4.1827069 0.0
*****
-0.0006731 6.05536 0.0
-0.00047595357441652345 6.055835953574417 0.0
0.0 6.0560331 0.0
*****
0.07552690000000001 6.13156 0.0
0.07572404642558347 6.132035953574417 0.0
0.0762 6.1322331 0.0
*****
0.22860000000000003 6.1322331 0.0
0.22907595357441654 6.132035953574417 0.0
0.2292731 6.13156 0.0
*****
0.47744634 6.06242374 0.0
0.47746294213947027 6.062431160364481 0.0
0.4774793600000001 6.06243898 0.0
*****
0.5225669000000001 6.13156 0.0
0.5227640464255835 6.132035953574417 0.0
0.52324 6.1322331 0.0
*****
0.7518400000000001 6.1322331 0.0
0.7523159535744166 6.132035953574417 0.0
0.7525131 6.13156 0.0
*****
2.32301542 6.10663498 0.0
2.3232331941927846 6.106781307383965 0.0
2.3234904000000003 6.1068331 0.0
*****
2.8391104 6.1068331 0.0
2.8394962006423152 6.106711677988141 0.0
2.8397428600000003 6.10639114 0.0
*****
3.22893182 6.13170732 0.0
3.2291685860022112 6.132085526306413 0.0
3.22958968 6.1322331 0.0
*****
3.5775696800000003 6.1322331 0.0
3.578045633574417 6.132035953574417 0.0
3.5782427800000005 6.13156 0.0
*****
3.58109266 6.11100124 0.0
3.5810981213636035 6.1109835689610295 0.0
3.5811028200000004 6.11096568 0.0
*****
3.5811028200000004 6.11096568 0.0
3.581097665305647 6.1109834386587565 0.0
3.58109266 6.11100124 0.0
*****
3.7292965800000006 6.13156 0.0
3.729493726425584 6.132035953574417 0.0
3.72996968 6.1322331 0.0
*****
3.9598600000000004 6.1322331 0.0
3.960335953574417 6.132035953574417 0.0
3.9605331000000006 6.13156 0.0
*****
4.0284882600000005 6.0564141000000005 0.0
4.02893295481865 6.056200340963728 0.0
4.029113100000001 6.055741 0.0
*****
4.029113100000001 0.1524 0.0
4.029061396913553 0.15214275684889197 0.0
4.02891498 0.15192502000000002 0.0
*****
3.87651498 -0.00047498 0.0
3.8762972058072154 -0.0006213073839646991 0.0
3.87604 -0.0006731 0.0
*****
3.7846 -0.0006731 0.0
3.784124046425583 -0.00047595357441670744 0.0
3.7839269 0.0 0.0
*****
3.1401131000000007 0.0 0.0
3.1399159535744174 -0.0004759535744167994 0.0
3.13944 -0.0006731 0.0
*****
2.9171773 -0.0006731 0.0
2.9168084710412754 -0.0005632027482395946 0.0
2.91656008 -0.00026924 0.0
*****
2.7781173800000003 -0.00026924 0.0
2.777869005845322 -0.0005632285560581688 0.0
2.7775001599999998 -0.0006731 0.0
*****
2.42062 -0.0006731 0.0
2.4201440464255835 -0.00047595357441661544 0.0
2.4199469000000002 0.0 0.0
*****
1.6084931 0.0 0.0
1.6082959535744166 -0.00047595357441666136 0.0
1.60782 -0.0006731 0.0
*****
1.1077092400000002 -0.0006731 0.0
1.1072699286841035 -0.0005096272777208597 0.0
1.10704376 -9.906e-05 0.0
*****
0.70143624 -9.906e-05 0.0
0.7012100848537824 -0.0005096429720839872 0.0
0.70077076 -0.0006731 0.0
*****
0.46099730000000005 -0.0006731 0.0
0.4606284711372198 -0.000563202601607623 0.0
0.4603800800000001 -0.00026924 0.0
*****
0.32193738 -0.00026924 0.0
0.32168900584532195 -0.000563228556058086 0.0
0.32132016 -0.0006731 0.0
*****
0.1524 -0.0006731 0.0
0.15214153574088737 -0.0006215323168355681 0.0
0.15192248 -0.00047498 0.0
*****

Thank you

[kandennti]

Hi @JeromeBriot .

It is very disappointing that it is still not fixed. It may be the SpurGear script that is most affected.

https://forums.autodesk.com/t5/fusion-360-api-and-scripts/gear-design/m-p/11675512 

For now, it seems that the only way is to use splines instead.

[JeromeBriot]

Thank you @kandennti. I searched the forum but didn't find this thread.

So this bug seems to be already reported as mentioned by @BrianEkins 

Hope it will be fixed soon.

[JeromeBriot]

Here is the code with the workaround by @jsugano_igears 

import adsk.core, traceback

p1 = [-0.00047752000000000005, 0.15192502000000002]
p2 = [-0.0006226001152828134,  0.15214303759958947]
p3 = [-0.0006731,              0.1524]

def run(context):

    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface

        product = app.activeProduct
        rootComp = product.rootComponent
        sketches = rootComp.sketches
        sketchesPlane = rootComp.xYConstructionPlane
        sketch = sketches.add(sketchesPlane)

        pt1 = adsk.core.Point3D.create(p1[0], p1[1], 0.0)
        pt2 = adsk.core.Point3D.create(p2[0], p2[1], 0.0)
        pt3 = adsk.core.Point3D.create(p3[0], p3[1], 0.0)

        # Fix by jsugano_igears
        # https://forums.autodesk.com/t5/fusion-360-api-and-scripts/gear-design/m-p/11679049/highlight/true#M18057
        try:

            sketch.sketchCurves.sketchArcs.addByThreePoints(pt1, pt2, pt3)

        except:

            tipArcPnts = adsk.core.ObjectCollection.create()
            tipArcPnts.add(pt1)
            tipArcPnts.add(pt2)
            tipArcPnts.add(pt3)

            sketch.sketchCurves.sketchFittedSplines.add(tipArcPnts)

        ui.messageBox('OK')

    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[MichaelT_123]

Hi Mr JeromeBriot,

It looks like you are messing around with old methods of gear teeth generators.😉

These methods utilize mapping a gear hobbing tool circular trajectory to the tooth profile. It is/was a natural approach as (in typical cases) gear cutting involves rotating tools, so approximation of the tooth profile by arc segments was a no-brainer at the time.  Splines, NURBS, and other goodies were not in the main circulation amongst machinists, and neither double precision computing like today but rather dwarf floats were in charge of virtual reality. Legacy gear generators are still part of today's software chain, and your example might be proof of it.

The idea of Mr. @jsugano_igears is valid, as describing a tooth profile as a spline offers many benefits (including precision). Of course, it depends upon your goal in the project.

You can also try the following:

1. Assemble a profile using Arc3D instead sketchArc. It might be faster. It would be interesting to check if your triplets are processed ... in the same way.
2. Use a sledgehammer approach bypassing F360 kernel and processing the data in, let's say, arbitral precision via, e.g. mpmath library.  

With Regards

MichaelT

[JeromeBriot]

---

@MichaelT_123 wrote:

It looks like you are messing around with old methods of gear teeth generators.😉

---

Actually, this is for my add-in IDF Import. A user reported a bug and I found that it was related to the addByThreePoints method. I have no control on the geometry because it is imported from files that are generated by external ECAD softwares.

[john.kirchner]

This issue has a fix that will be released in next month's update - thank you for posting a workaround!

[kandennti]

What's New says the "SketchArcs.addByThreePoints" method is fixed.

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-36B1FFB5-5291-4532-8F11-90E912769B34 

However, I still get an error when I try it. (Ver 2.0.16265)

This is what I tried when this topic was created.

# Fusion360API Python script
import traceback
import adsk.core as core
import adsk.fusion as fusion
def run(context):
    ui: core.UserInterface = None
    try:
        app: core.Application = core.Application.get()
        ui = app.userInterface
        des: fusion.Design = app.activeProduct
        root: fusion.Component = des.rootComponent
        p1: core.Point3D = core.Point3D.create(0.1524, -0.0006731, 0.0)
        p2: core.Point3D = core.Point3D.create(0.15214153574088737, -0.0006215323168355681, 0.0)
        p3: core.Point3D = core.Point3D.create(0.15192248, -0.00047498, 0.0)

        skt: fusion.Sketch = root.sketches.add(root.xYConstructionPlane)

        # sketchCircles.addByThreePoints - OK
        skt.sketchCurves.sketchCircles.addByThreePoints(p1, p2, p3)

        # sketchArcs.addByThreePoints - Error
        skt.sketchCurves.sketchArcs.addByThreePoints(p1, p2, p3)

    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

At that time (one month ago), "SketchArcs.addByThreePoints" failed, but "sketchCircles.addByThreePoints" worked fine.
Unfortunately, in ver. 2.0.16265, "sketchCircles.addByThreePoints" also fails.
The situation is getting worse.

[BrianEkins]

It's strange because the specific case causing the spur gear to fail is now working. However, this simpler case now fails. I can reproduce this in the UI by drawing two points 0.01 mm apart and then trying to create an arc or circle using those points. This is a new problem with the May release, and I've reported it. Hopefully, it's fixed soon.

[kandennti]

Thank you @BrianEkins  for confirming this.

[JeromeBriot]

This bug has resurfaced... 

import adsk.core, traceback

p1 = [30.080034000086005, 8.520248200008002]
p2 = [30.080018452397404, 8.52024309287324]
p3 = [30.080002900072003, 8.520237999876]

# The code works with f = 100
f = 1

def run(context):

    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface

        product = app.activeProduct
        rootComp = product.rootComponent
        sketches = rootComp.sketches
        sketchesPlane = rootComp.xYConstructionPlane
        sketch = sketches.add(sketchesPlane)

        pt1 = adsk.core.Point3D.create(p1[0]*f, p1[1]*f, 0.0)
        pt2 = adsk.core.Point3D.create(p2[0]*f, p2[1]*f, 0.0)
        pt3 = adsk.core.Point3D.create(p3[0]*f, p3[1]*f, 0.0)

        # Fix by jsugano_igears
        # https://forums.autodesk.com/t5/fusion-360-api-and-scripts/gear-design/m-p/11679049/highlight/true#M18057
        try:

            sketch.sketchCurves.sketchArcs.addByThreePoints(pt1, pt2, pt3)
            
            ui.messageBox('sketchCurves.sketchArcs.addByThreePoint OK')

        except:

            tipArcPnts = adsk.core.ObjectCollection.create()
            tipArcPnts.add(pt1)
            tipArcPnts.add(pt2)
            tipArcPnts.add(pt3)

            sketch.sketchCurves.sketchFittedSplines.add(tipArcPnts)

            ui.messageBox('sketchCurves.sketchFittedSplines OK')
        
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[BrianEkins]

Do you know when it quit working? Did these same three points work OK before? I checked the points without any scaling, and the point that is between the other two is only 

7.43924394585801e-09 cm from a line connecting the two other points. I don't know what the tolerance is before Fusion considers the points to be colinear, but it wouldn't surprise me if this is in that range. Two points are considered equal if they are within 1e-06 cm to each other.

[JeromeBriot]

@BrianEkins The issue was reported by a user of the Import IDF add-in yesterday.

You're right about the tolerance. I think I'll have to incorporate the spline workaround into my code this time.

[JeromeBriot]

My apologies.

In fact, I have already patched my code with the workaround but a duplicate section was left unmodified.

I have replaced these two sections with a function that includes the workaround.

I submitted the new version of the add-in yesterday.