Macro Failing to Create Circle

Discussion created by Jorge Mirabelli on Aug 6, 2019
Latest reply on Aug 6, 2019 by Jorge Mirabelli

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I have a macro that works about 60% of the time and I have no idea why. I will run it with the same data three times and get three different results, please help. The line which fails is:

Set skSegment = Part.SketchManager.CreateCircleByRadius(xValue, yValue, zValue, Range("D" & i).Value / 1000)

where I am just trying to create a circle using variables that are storing the center's data. What is strange is that sometimes if I add a break point at this line and do NOTHING except click the continue button the code will work...at least on my computer. I am now on a better computer but it is failing more frequently. I have watched the variables used in the expression and they always are valid numbers. Unfortunately the upload video feature is currently down, but what happens is the blue circle and orange coordinate axes will flash on the screen for a moment and then disappear and no circle will have been created despite the sketch having attempted to create one. Sorry if this doesn't really make sense, I do not know how to explain it...

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Jacob Corder Aug 6, 2019 11:01 AM

add this code to see if it fixes it.

add it to where you put the breakpoint

the code is DoEvents add it right before Set SkSegment = Part.SketchManager.CreateCircleByRadius(xValue, yValue, zValue, Range("D" & i).Value / 1000)

like this

DoEvents

Set skSegment = Part.SketchManager.CreateCircleByRadius(xValue, yValue, zValue, Range("D" & i).Value / 1000)

post the code if you need further help

also use the new API

https://help.solidworks.com/2019/english/api/sldworksapi/SOLIDWORKS.Interop.sldworks~SOLIDWORKS.Interop.sldworks.IModelDoc2~ICreateCircleByRadius2.html
also read the information in this link

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Jorge Mirabelli @ Jacob Corder on Aug 6, 2019 11:51 AM

Thanks for the attempt, unfortunately it did not work, but while I was trying it I found out that the failing is due to my view! I have not figured out why exactly where I position my view has anything to do with creating a circle at a given point or what view allows which circles to be sketched. I attached the entire code (core generation vba) and specifically the macro that is causing me trouble (Draw Circles vba). Line 51 is the sketch circle line.

I must also give credit to Peter Simpson for the original code that I added onto (I added the draw splines and draw circles commands for clarification).

I appreciate your help Jacob.

Attachments

Draw Circles vba.docx12.9 KB
core generation vba.docx16.6 KB

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Josh Brady @ Jorge Mirabelli on Aug 6, 2019 12:03 PM

I haven't looked at your code... But this symptom is almost always caused by not turning on AddToDB. When you create sketch entities through API, it actually creates as though you clicked that point. So, automatic relations, snaps, etc. try to happen. If your zoom level is wrong, it will not create things because it clicks the same point twice, or it will make unexpected relations or snaps. Using AddToDB (SetAddToDB? If forget...) turns off all that snapping.

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Simon Turner @ Jorge Mirabelli on Aug 6, 2019 12:05 PM

You are missing the line:

Part.SketchManager.AddToDB = True

this forces SolidWorks to create your sketch geometry exactly where you are asking it to. Without that line, it will snap to any point that is near the desired point, depending on the view you are in.

Don't forget to turn AddToDB off after creating the sketch elements:

Part.SketchManager.AddToDB = False

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Jorge Mirabelli @ Simon Turner on Aug 6, 2019 12:18 PM

Does that have to be right before the circle is made or before the sketch is created/inserted?

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Simon Turner @ Jorge Mirabelli on Aug 6, 2019 12:23 PM

Before the creation of any sketch geometry, but after the sketch creation.

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Jorge Mirabelli @ Simon Turner on Aug 6, 2019 12:42 PM

Another quick question, I currently have hard written into the code to use 3DSketch2 when it begins drawing planes and circles based on points in 3DSketch2. How do I change the code so that it uses whichever sketch I have selected?

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Jorge Mirabelli Aug 6, 2019 12:16 PM

Thank you all for your help and teaching me about the AddToDB command...will be useful in the future!

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8 Replies

Jacob Corder Aug 6, 2019 11:01 AM
add this code to see if it fixes it.
add it to where you put the breakpoint

the code is DoEvents add it right before Set SkSegment = Part.SketchManager.CreateCircleByRadius(xValue, yValue, zValue, Range("D" & i).Value / 1000)

like this

DoEvents
Set skSegment = Part.SketchManager.CreateCircleByRadius(xValue, yValue, zValue, Range("D" & i).Value / 1000)

post the code if you need further help

also use the new API
https://help.solidworks.com/2019/english/api/sldworksapi/SOLIDWORKS.Interop.sldworks~SOLIDWORKS.Interop.sldworks.IModelDoc2~ICreateCircleByRadius2.html
also read the information in this link
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- Jorge Mirabelli @ Jacob Corder on Aug 6, 2019 11:51 AM
  Thanks for the attempt, unfortunately it did not work, but while I was trying it I found out that the failing is due to my view! I have not figured out why exactly where I position my view has anything to do with creating a circle at a given point or what view allows which circles to be sketched. I attached the entire code (core generation vba) and specifically the macro that is causing me trouble (Draw Circles vba). Line 51 is the sketch circle line.
  
  I must also give credit to Peter Simpson for the original code that I added onto (I added the draw splines and draw circles commands for clarification).
  
  I appreciate your help Jacob.
  Attachments
  - Draw Circles vba.docx12.9 KB
  - core generation vba.docx16.6 KB
  Like • Show 0 Likes0
  Actions
  - Josh Brady @ Jorge Mirabelli on Aug 6, 2019 12:03 PM
    I haven't looked at your code... But this symptom is almost always caused by not turning on AddToDB. When you create sketch entities through API, it actually creates as though you clicked that point. So, automatic relations, snaps, etc. try to happen. If your zoom level is wrong, it will not create things because it clicks the same point twice, or it will make unexpected relations or snaps. Using AddToDB (SetAddToDB? If forget...) turns off all that snapping.
    Like • Show 0 Likes0
    Actions
  - Simon Turner @ Jorge Mirabelli on Aug 6, 2019 12:05 PM
    You are missing the line:
    Part.SketchManager.AddToDB = True
    this forces SolidWorks to create your sketch geometry exactly where you are asking it to. Without that line, it will snap to any point that is near the desired point, depending on the view you are in.
    Don't forget to turn AddToDB off after creating the sketch elements:
    Part.SketchManager.AddToDB = False
    Like • Show 0 Likes0
    Actions
    - Jorge Mirabelli @ Simon Turner on Aug 6, 2019 12:18 PM
      Does that have to be right before the circle is made or before the sketch is created/inserted?
      Like • Show 0 Likes0
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      - Simon Turner @ Jorge Mirabelli on Aug 6, 2019 12:23 PM
        Before the creation of any sketch geometry, but after the sketch creation.
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        Jorge Mirabelli @ Simon Turner on Aug 6, 2019 12:42 PM
        Another quick question, I currently have hard written into the code to use 3DSketch2 when it begins drawing planes and circles based on points in 3DSketch2. How do I change the code so that it uses whichever sketch I have selected?
        Like • Show 0 Likes0
        Actions
Jorge Mirabelli Aug 6, 2019 12:16 PM
Thank you all for your help and teaching me about the AddToDB command...will be useful in the future!
Like • Show 0 Likes0
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Macro Failing to Create Circle

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