FreeCAD/C3/Fixing-the-Wire-is-not-Closed-Error/English

Title of the script: Fixing the Wire is not Closed Error in FreeCAD

Author: Chitra Balaji.

Keywords: FreeCAD, Missing coincidence, Validate Sketch tool, Pad tool,

Overlapping lines, video tutorial.

Visual Cue	Narration
Slide 1 Title Slide	Welcome to this Spoken Tutorial on Fixing the Wire is not Closed Error in FreeCAD.
Slide 2 Learning Objectives	In this tutorial, we will learn to: Understand the wire is not closed error in FreeCAD. Identify gaps or overlapping lines in a sketch using the Validate sketch tool. Fix the error and pad the sketch.
Slide 3 System Requirements	To record this tutorial, I am using: Windows 11 and FreeCAD version 1.0.0
Slide 4 Prerequisite	To follow this tutorial, Learners should have basic knowledge of the FreeCAD interface.
Right click on the Freecad app image, Select Run.	Let’s open the FreeCAD interface.
Click on File menu select the new option Go to File and click New.	Let us open a new file.
Switch to Part Design Workbench. Click on the Create sketch tool Under the Tasks panel, Select attachment as XY-plane and click OK.	Let us select Part Design Workbench.Then click the Create Sketch tool. Under the Tasks panel, Select attachment as XY-plane and click OK.
Rectangle tool highlighted in Sketcher. Select one corner and drag the mouse Press Esc key to deselect the Rectangle tool. Or Right-click on the interface. Highlight the red corner points.	In the sketch, select the Rectangle tool. Draw a rectangle. Press Esc key to deselect the Rectangle tool. Let's trigger the wire is not closed error by deleting one coincidence constraint.
Constraints panel shows the constraint coincidences selected. (Constraints 1, Constraints 2, Constraints 3 etc,.) Press the Delete key on the Keyboard. Highlight the corner points	Select one Coincidence constraint from the left panel. Press the Delete key on the keyboard. Notice that the rectangle’s corner point turns from red to white colour. Now the lines connecting the endpoint are free to move.
Zoom in the corners of the rectangle using the mouse wheel. Highlight the lines Press the endpoint of the line and Move the line Zoom the sketch using mouse Click on the endpoint where the yellow dot appears and move little.	Zoom in to see the endpoints of the lines. Click on one of the endpoints. Move it slightly so that the endpoints no longer meet.
Click the close button on the left panel Pad tool seen in part design pad Pad tool highlighted Click ok Error message is displayed Click ok on the message Click the Cancel button on the left side to cancel the padding.	Close the sketch. Click the Pad tool. Pad parameters box opens. Click OK. Input error message, Wire is not closed appears and the sketch is not padded. Click OK in the pop-up message. Click the Cancel button in the left panel to cancel the padding.
Click the model tab under the model tree. Click the sketch Click on the Validate Sketch Tool on the tool bar. Sketcher validation dialog box opens. Click Highlight Troublesome Vertices Point to the highlighted disconnected endpoints. Zoom the sketch using mouse	To fix this error, select the sketch in the Model tree. Click on the Validate Sketch Tool on the tool bar. Sketcher validation dialog box opens in the left panel. Click Highlight Troublesome Vertices. This will highlight the disconnected endpoints. This tool helps to check for gaps, overlaps, and other geometry errors.
Click on Missing Coincidences and click find Tolerance box is highlighted Select the value in the dropdown box Click on the Find button. Click Fix Button. Click ok Highlight the fix button Zoom to see the endpoints	Under Missing coincidences, Select the tolerance value as 0.01. Tolerance defines how close two vertices must be to count as coincident. Click on the Find button. If the Fix button is active, click on it to reconnect the endpoints. Then Click OK. In some cases, the fix button is not active as shown. This is because the distance between the two points should be less than the tolerance value for the Fix tool to work. In that case fixing the endpoints has to be done manually.
Click Highlight Troublesome Vertices. Show the highlighted points. Go to sketch Click the Coincidence constraint icon from the toolbar.	Click Highlight Troublesome Vertices. This will highlight the disconnected endpoints. Note the highlighted points. Click on Close Go to sketch select the two points that need to be joined. Click the Coincidence constraint icon from the toolbar. Note that the points are connected. Click on Close
Click the Pad tool from the tool bar. Click OK button	Now lets select the Pad tool. Click the OK button. We can see the sketch is padded now.
Another common 'wire is not closed' error is caused by overlapping lines. Lets do that in assignment
Slide 5 Summary In this tutorial, we have learnt to: Understand the Wire is not closed error in FreeCAD. Identify gaps or overlapping lines in a sketch using the Validate sketch tool Fix the error and pad the sketch.	With this, we come to the end of this tutorial. Let us summarize.
Slide 6 Assignment In Sketcher, draw a rectangle. Add a line over one rectangle edge. Close the sketch and try padding. If an error occurs, reopen the sketch. Use Validate Sketch tool to find overlaps. Delete the extra line and close sketch. Check if padding works.	As an assignment, please do the following:
Slide 7 Thank you	Thank you for joining.

Contributors and Content Editors

Ketkinaina, Madhurig