Sketch with text via API not exporting text but will manually

[marylou.forsyth]

Good day programmers!  I am asking for help as I am just not seeing what steps I am missing.  Please let me give the background.  We open a model via API script, we read in new parameters to update the model to, and update the model.  All processing is done via the API script.  My customer has requested a specific type of processing done, where the model has a few sketches, to delete all sketches not named in a list, and export the model as a DXF.  The logic I wrote to address this can be identified as the DXF_Type_BPB (for it needs to be a DXF export with only the Body, Pen_lines and Bend_Lines {BPB})

The logic goes through and removes the sketches not needed, then exports out a file with just the pen-line (so I can verify in testing which actually looks great) and then exports out the body and the one sketch Pen_Line.  My problem is when the second export happens, I don't see the text.  

The manual export (fullPath + sketch.name + 'dxf') which is looking ok to me appears as this:

and at the top you can see the text data 'HV something'.

The export with the body, Pen_line though only creates this as I must be missing something major:

Here is the code (please ignore the section that says else: DXF_Type_BPB == False ) AND please forgive the horrible loop where I flush out the un-needed sketches, it will be re-written.

I thought this line was going to give what I needed but sadly no:

[sketchEntities.add(ent) for ent in sketch.sketchTexts]

One more thing, there is logic to adjust the scaling but thats been working fine.  

#we call this right before the code in question --> : updateParametricModel(tag,value,userParams,False)

else: # its a punch so export the drawing scaled correctly
global DXF_Type_BPB
# flag if problem of no cam found when making a DXF
Stop_it = False

folder = "W:\\SharedData\\Fusion_360\\DXF\\"
fullPath = os.path.join(folder, order)

if (DXF_Type_BPB == True):
Total_Count_Sketches = 0
targetSketches = ['Pen_Line','Pen_line','pen_line','Bend_Line','Bend_line','bend_line']
DFX_Generated = True
design : adsk.fusion.Design = app.activeProduct
root: adsk.fusion.Component = design.rootComponent
master: adsk.fusion.Sketch = root.sketches.add(root.xYConstructionPlane)
rootComp: adsk.fusion.Component = design.rootComponent

#### Check names of all sketches
#sketches = rootComp.sketches
#sketch_names = []
#i1 = 0
#for sk in sketches:
# print(str(sketches.item(i1).name))
# i1 = i1 + 1
#####

sketches = rootComp.sketches
sketch_names = []
Kludge_Counter = 0
Not_done = False
while Not_done == False:
Kludge_Counter = Kludge_Counter + 1
if (Kludge_Counter > 20):
Not_done = True
i1 = 0
for sk in sketches:
sketch = sketches.item(i1)
if (sketch.name in targetSketches):
#sketch_names.append(sketches.item(i1).name)
print(str(sketches.item(i1).name))
i1 = i1 + 1
else:
print(str(sketches.item(i1).name))
sketch.deleteMe()
break
# This matches the manually exported DXF,
# so things are great up to here ...I think...
sketch.saveAsDXF(fullPath + sketch.name + '.dxf')

####
sketches = rootComp.sketches
sketch_names = []
i1 = 0
for sk in sketches:
print(str(sketches.item(i1).name))
# nope master.project(sk)
i1 = i1 + 1
#####

sketchEntities: adsk.core.ObjectCollection = adsk.core.ObjectCollection.create()
for sketch in rootComp.sketches:
myname = sketch.name
print(myname)
[sketchEntities.add(ent) for ent in sketch.sketchCurves]
[sketchEntities.add(ent) for ent in sketch.sketchPoints]
[sketchEntities.add(ent) for ent in sketch.sketchTexts]

# Create new Sketch
master: adsk.fusion.Sketch = rootComp.sketches.add(rootComp.xYConstructionPlane)
master.name = 'Master'
# Project Body
targetBody: adsk.fusion.BRepBody = rootComp.bRepBodies[0]
project_result: adsk.core.ObjectCollection = master.project(targetBody)
if project_result.count < 1:
print('Failure of the body project')

# Include sketchEntities
master.include(sketchEntities)

# Project sketchEntities
master.project(sketchEntities)

else: # (DXF_Type_BPB == False)
design : adsk.fusion.Design = app.activeProduct
# new logic 2 statements added 02-28-2023
document = app.activeDocument
design = document.design
try:
rootComp = design.rootComponent
except:
msg = 'This model contains no CAM object, no DXF can be generated'
if (run_from_list == False):
# inform operator issue no cam object found
ui.messageBox(msg)
Stop_it = True
_flags.append(msg)
else:
# set a flag so we skip all further processing
Stop_it = True
print(msg)

if (Stop_it == False):
master: adsk.fusion.Sketch = rootComp.sketches.add(rootComp.xYConstructionPlane)
targetBody: adsk.fusion.BRepBody = rootComp.bRepBodies[0]
master.project(targetBody)

if (Stop_it == False):
# Scale the model if its in inches
if(in_inches == True):
basePt = master.sketchPoints.item(0)
scaleFactor = adsk.core.ValueInput.createByString("10 mm")
#scales = rootComp.features.scaleFeatures
scales = rootComp.features.scaleFeatures
#Create an uniformed input for scale feature input
inputUniformColl = adsk.core.ObjectCollection.create()
inputUniformColl.add(master)
scaleUniformInput = scales.createInput(inputUniformColl, basePt, scaleFactor)
scaleUniform = scales.add(scaleUniformInput)

# Special scaling for the other tool for MM models, updated 12-8-22
if(in_inches == False):
basePt = master.sketchPoints.item(0)
scaleFactor = adsk.core.ValueInput.createByString("1.0 in/64.516")
#scales = rootComp.features.scaleFeatures
scales = rootComp.features.scaleFeatures
#Create an uniformed input for scale feature input
inputUniformColl = adsk.core.ObjectCollection.create()
inputUniformColl.add(master)
scaleUniformInput = scales.createInput(inputUniformColl, basePt, scaleFactor)
scaleUniform = scales.add(scaleUniformInput)

# write the merged file
master.saveAsDXF(fullPath + '.dxf')
msg = '!! DXF file has been written !!'
DFX_Generated = True
#print(msg)
futil.log(msg)

I will drag and drop as this is hard to read.

Thank you for your time and assistance, I have looked and tried so many different things but I just can't resolve this.

[kandennti · Accepted solution]

Hi @marylou.forsyth .

If you want to include your code in the forum, this is a good way to display it.

When I tried, the project/include method was not available for SketchText objects.

Therefore, I created a sample that explodes and then projects the data.

# Fusion360API Python script

import traceback
import adsk.core as core
import adsk.fusion as fusion

def run(context):
    ui = core.UserInterface.cast(None)
    try:
        app: core.Application = core.Application.get()
        ui = app.userInterface
        des: fusion.Design = app.activeProduct
        root: fusion.Component = des.rootComponent

        path = r'C:\temp\test.dxf'

        targetSketchNames = ['PEN_LINE','BEND_LINE']

        try:
            app.executeTextCommand(u'Transaction.Start export_project_sketch')

            export_project_sketch(
                targetSketchNames,
                root.xYConstructionPlane,
                path,
            )
        except:
            pass
        finally:
            app.executeTextCommand(u'Transaction.Abort')

        ui.messageBox('Done')

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


def export_project_sketch(
    targetSketchNames: list,
    supportPlane: fusion.ConstructionPlane,
    path: str,
) -> None:

    def get_sketch_entities(
        skt: fusion.Sketch,
    ) -> list:

        lst = [c for c in skt.sketchCurves]
        lst.extend([p for p in skt.sketchPoints])

        return lst

    def explode_sketchTexts(
        skt: fusion.Sketch,
    ) -> None:

        skt.isComputeDeferred = True

        sktTxtLst = [t for t in skt.sketchTexts]
        [t.explode() for t in sktTxtLst]
            
        skt.isComputeDeferred = False
    # *******

    app: core.Application = core.Application.get()
    des: fusion.Design = app.activeProduct
    root: fusion.Component = des.rootComponent

    sktLst = [skt for skt in root.sketches if skt.name.upper() in targetSketchNames]
    if len(sktLst) < 1:
        return

    [explode_sketchTexts(skt) for skt in sktLst]

    sktEnts = []
    [sktEnts.extend(get_sketch_entities(skt)) for skt in sktLst]
    if len(sktEnts) < 1:
        return

    sketchEntities: core.ObjectCollection = core.ObjectCollection.create()
    [sketchEntities.add(e) for e in sktEnts]

    master: fusion.Sketch = root.sketches.add(supportPlane)
    master.name = 'Master'

    master.project(sketchEntities)
    master.saveAsDXF(path)

Since it would be inconvenient if the original data were left exploded, we used a transaction of text commands to return the data to the state before processing.
However, since explode is very time-consuming, I do not think it will be useful in practice.

[marylou.forsyth]

You are a wonder to behold!  You have nailed the issue, I have been working on this and you just brought it to a resolution, bless you!!  Yes, so right you are I spoke with the developers and they will explode the text in sketches so the API will not have too.  Would not have gotten here without your help, thank you!!