make centermark with Ilogic
Can you please provide non confidential data and screenshot of centermark which is created manually or UI?
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network
Hi @Darkforce_the_ilogic_guy did you solved?
Admaiora
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Great work @tdant
Thanks for sharing!
Admaiora
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Try this. You would have to make sure your AutomatedCenterLineSettings are where you want them (which I believe could also be done within iLogic), but this should do what you want. It doesn't delete any center marks that may already be there, but it's a good start. Let me know how it works for you.
Dim oDoc As DrawingDocument = ThisDrawing.Document Dim oSheet As Sheet = oDoc.ActiveSheet Dim oViews As DrawingViews = oSheet.DrawingViews Dim oViewOrient As ViewOrientationTypeEnum Dim oACS As AutomatedCenterlineSettings Dim oCLs As ObjectsEnumerator For Each oView As DrawingView In oViews oViewOrient = oView.Camera.ViewOrientationType If oViewOrient = ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation Then Return ElseIf oViewOrient = ViewOrientationTypeEnum.kIsoBottomRightViewOrientation Then Return ElseIf oViewOrient = ViewOrientationTypeEnum.kIsoTopLeftViewOrientation Then Return ElseIf oViewOrient = ViewOrientationTypeEnum.kIsoTopRightViewOrientation Then Return Else oView.GetAutomatedCenterlineSettings(oACS) oACS.ApplyToBends = False oACS.ApplyToCircularPatterns = True oACS.ApplyToCylinders = False oACS.ApplyToFillets = False oACS.ApplyToHoles = True oACS.ApplyToPunches = True oACS.ApplyToRectangularPatterns = True oACS.ApplyToRevolutions = False oACS.ApplyToSketches = False oACS.ApplyToWorkFeatures = False 'oACS.ArcAngleThreshold = 'oACS.CircularEdgeMaximumThreshold = 'oACS.CircularEdgeMinimumThreshold = 'oACS.FilletRadiusMaximumThreshold = 'oACS.FilletRadiusMinimumThreshold = oACS.ProjectionNormalAxis = True oACS.ProjectionParallelAxis = True 'oACS.RadiusThresholdPrecision = oCLs = oView.SetAutomatedCenterlineSettings(oACS) End If Next
Wesley Crihfield
(Not an Autodesk Employee)
Could you please help with an iLogic rule for only the outside circle, as shown in the photo below?
@DIMCWPDR , you can right click on the outer circle and use Capture Current State as shown below, and then use the iLogic Centermark snippet to do this:
Hi @DIMCWPDR. That is not very much information to go by.
In order for any code to only create one Centermark, when there are multiple circles involved that would normally also get Centermarks, there would need to either be some manual user selection involved, or some very specific design information included within the code, such as circle radius / diameter upper and lower limits, and maybe even knowing exactly what type of feature that the circle represents. So, would it be OK if the code asked you to pick that outer circle first, then place a Centermark on it by code after that? If so, then there would not really be much need for the code to automate it, because the same can be done manually easier. If you do not want to have to manually select that outer circle, then how else would one of us be able to find that outer circle by code when we know nothing about it? We would need a lot more information than that to go on, such as an actual example drawing (with model being referenced in its views), or maybe a lot more details about the types of features and their sizes. Explaining why this is needed may help also. For example, we don't want to spend an hour writing code for something that will only be used once, in one drawing, then never used for anything else ever again, because it is far too specific.
You can review the online help pages for the Inventor API stuff in the links below for more insight into what is needed to create Centermarks on a sheet in a drawing.
Centermarks.AddByCenterOfGravity
DrawingView.GetAutomatedCenterlineSettings
DrawingView.SetAutomatedCenterlineSettings
Wesley Crihfield
(Not an Autodesk Employee)
Hallo curtis waguespack
I think I need help again with mig ilogic code. I need only the centermatks only as shown in the pic below:
But when i run the rule i get the centermark in all the holes.
Can you please tell me which the text i have to tuen off or remove?
Her is the rule:
Dim oDoc As DrawingDocument = ThisDrawing.Document Dim oSheet As Sheet = oDoc.ActiveSheet Dim oViews As DrawingViews = oSheet.DrawingViews Dim oACS As AutomatedCenterlineSettings Dim oCLs As ObjectsEnumerator For Each oView As DrawingView In oViews If oViewOrient = ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation Then Return Else oView.GetAutomatedCenterlineSettings(oACS) oACS.ApplyToBends = False oACS.ApplyToCircularPatterns = True oACS.ApplyToCylinders = False oACS.ApplyToFillets = False oACS.ApplyToPunches = True oACS.ApplyToRectangularPatterns = True oACS.ApplyToRevolutions = False oACS.ApplyToSketches = False oACS.ApplyToWorkFeatures = False oACS.ProjectionNormalAxis = True oACS.ProjectionParallelAxis = True CLs = oView.SetAutomatedCenterlineSettings(oACS) End If Next Dim Sheet_1 = ThisDrawing.Sheets.ItemByName("Sheet:1") Dim VIEW1 = Sheet_1.DrawingViews.ItemByName("VIEW1") Dim Face0 = VIEW1.GetIntent("Face0", PointIntentEnum.kCenterPointIntent) Dim centermark = Sheet_1.Centermarks.Add("Hole Centermark", Face0)
Hi @DIMCWPDR. As I mentioned in message 10 above, if you want to use the AutomatedCenterlineSettings for these types of tasks, then you would have to customize those settings according to the size of the feature you are targeting, and by what type of feature created it. Review the following copy of your last code, and my comments on some of those lines. If we know what type of feature created that largest round circular feature, then we can filter out all other types of features, leaving only that type of feature. Also, your images do not indicate what size the largest circles are, or what size the smaller circles are, so only you would know that. There are settings for minimum and maximum radius to be considered for getting things like centerlines and centermarks. But we can not write those values in for you, because we can not tell now small to make the minimums, and how large to make the maximums.
Also note the changes I made to the 'If' statement just inside the loop of views. It should now filter out any view set to that one specific view orientation, but when that one is encountered, it will now continue on to the next view, if any, instead of exiting out of the whole rule. I also eliminated the last several lines, because they had no use anymore in this example.
Dim oDoc As DrawingDocument = ThisDrawing.Document
Dim oSheet As Sheet = oDoc.ActiveSheet
Dim oViews As DrawingViews = oSheet.DrawingViews
Dim oACS As AutomatedCenterlineSettings
Dim oCLs As ObjectsEnumerator
For Each oView As DrawingView In oViews
If oView.Camera.ViewOrientationType = ViewOrientationTypeEnum.kIsoBottomLeftViewOrientation Then
Continue For
Else
oView.GetAutomatedCenterlineSettings(oACS)
'if you know the size of the largest radius, then set these next two settings
'set Max circular Radius (in centimeters) to get a centerline / centermark
oACS.CircularEdgeMaximumThreshold = 100
'set Min circular Radius (in centimeters) to get a centerline / centermark
oACS.CircularEdgeMinimumThreshold = 2
'set Max fillet radius (in centimeters) to get a centerline / centermark
oACS.FilletRadiusMaximumThreshold = 20
'set Min fillet radius (in centimeters) to get a centerline / centermark
oACS.FilletRadiusMinimumThreshold = 2
oACS.ApplyToBends = False
oACS.ApplyToCircularPatterns = False
'if they were created using Hole feature, this would effect them
oACS.ApplyToHoles = False
'this next one would apply to all cylindrical faces
oACS.ApplyToCylinders = False
oACS.ApplyToFillets = False
oACS.ApplyToPunches = False
oACS.ApplyToRectangularPatterns = False
'If the feature was created using Revolve feature
oACS.ApplyToRevolutions = True
oACS.ApplyToSketches = False
oACS.ApplyToWorkFeatures = False
oACS.ProjectionNormalAxis = True
oACS.ProjectionParallelAxis = True
CLs = oView.SetAutomatedCenterlineSettings(oACS)
End If
Next
Wesley Crihfield
(Not an Autodesk Employee)
Hi @DIMCWPDR. Here is also another code example which uses Inventor API and shows how a centermark can be added to a circular curve within a drawing view. This example requires you to manually select the circular geometry within the view, then it will add the centermark for you. Just as additional information about situations like this.
Dim sPrompt As String = "Pick a circular drawing view curve to add centermark to, or press ESC key to exit."
Dim oFilter = SelectionFilterEnum.kDrawingCurveSegmentFilter
Dim oPickedDCS As DrawingCurveSegment = ThisApplication.CommandManager.Pick(oFilter, sPrompt)
If oPickedDCS Is Nothing Then
MsgBox("Nothing Selected, so exiting rule.", vbInformation, "iLogic")
Return
End If
Dim oDCurve As DrawingCurve = oPickedDCS.Parent
Dim oView As DrawingView = oDCurve.Parent
Dim oSheet As Inventor.Sheet = oView.Parent
'Dim oDDoc As DrawingDocument = oSheet.Parent
If oPickedDCS.GeometryType = Curve2dTypeEnum.kCircleCurve2d OrElse
oDCurve.CurveType = CurveTypeEnum.kCircleCurve Then
Dim oGeomIntent As GeometryIntent = oSheet.CreateGeometryIntent(oDCurve, PointIntentEnum.kCenterPointIntent)
oSheet.Centermarks.Add(oGeomIntent, True)
Else
MsgBox("Selected Geometry was not a circle, so nothing happens.", vbInformation, "iLogic")
Return
End IfWesley Crihfield
(Not an Autodesk Employee)
We can definitely write code that will apply centermarks to pretty much anything in every drawing view that is capable of getting a centermark placed on it. However, if you only want certain specific things to get them, and not others, that is where the complication comes in. We simply need a way to identify the specific geometry that you want to get centermarks, and a way to identify the specific geometry that would normally also get a centermark, but you do not want them to get centermarks, such as the circular pattern of holes in that part. The code we write must be extremely specific or it will not work, so without extremely specific information (from you or a sample drawing), that can be nearly impossible to write the code for.
In the earlier example that used 'Capture Current State', that uses powerful iLogic functionality (that we users do not have the source code for) to actually assign a generic name to the geometry in the model that the selected view geometry represents. Then we can use that name later in the code, to help identify that specific piece of geometry, for things like GeometryIntent, which is used for attaching annotations to view geometry. However, what most folks do who want to automate their drawings is, prepare their models ahead of time, by assigning specific names to all the pieces of geometry that they will want to attach drawing dimensions and / or other drawing annotations to in the drawing later. Then when in the drawing later, they can find those specific pieces of geometry within their views using the names that they assigned to them in the model. In the examples above, we do not know if you have assigned any names to any of that geometry in your model, so we just assumed that you had not done that yet. But that would make situations like this much easier to manage. It gives you more control over being able to find and use specific view geometry for attaching dimensions and annotations to them in your drawing. Without that we are 'flying blind' so to speak. I hope you understand what I mean with all of this.
In a part, you can select a Face, Edge, or Vertex, then right-click, and within the right-click menu will be an option named 'Assign Name...'. That is where you assign names to geometry, so you can easily find it again later by code. We can also assign names to stuff by code, using Attributes, which is what that system uses behind the scenes. But assigning names to geometry should be done by someone who is extremely familiar with what that geometry is, so that the names are most meaningful to them, so they know which ones are which later.
Wesley Crihfield
(Not an Autodesk Employee)
Can I provide you with my .ipt and .idw files so you can take a look at them? The problem is that I have many gasket drawings like this for my project, and I need to automatically generate centerlines and centermarks as shown below
I only need this centerlins as following pic below
