Difference between revisions of "FreeCAD/C3/Introduction-to-Part-Design-Workbench/English"

From Script | Spoken-Tutorial
Jump to: navigation, search
 
Line 261: Line 261:
 
|| Select the vertical line.
 
|| Select the vertical line.
  
−
Select '''Constrain vertical distance tool.'''
+
Select '''Constrain vertical distance tool'''.
  
 
Fill the '''Length '''field as 30 mm.
 
Fill the '''Length '''field as 30 mm.
Line 356: Line 356:
 
Select the '''Create circle''' tool and place the cursor on the x-axis.
 
Select the '''Create circle''' tool and place the cursor on the x-axis.
  
−
You can see that line changes to a yellow color.
+
You can see that line changes to yellow color.
  
 
You can see that '''Constrain point onto object''' symbol appears near the cursor.  
 
You can see that '''Constrain point onto object''' symbol appears near the cursor.  

Latest revision as of 12:52, 11 July 2024

Title of script: Introduction to Part Design Workbench.

Author: Dr. Sathiya Narayanan, K.Sakthivel.

Keywords: FreeCAD, Part Design, Sketcher workbench, Sketcher tools, constrains, pad tool, pocket tool, video tutorial.


Visual Cue Narration
Slide 1

Title slide

Welcome to this Spoken Tutorial on Introduction to Part Design Workbench.
Slide 2

Learning Objectives

In this tutorial, we will learn to,
  • Draw basic shapes.
  • Use basic constrains.
  • Draw the Flange Coupling component in 3D.
Slide 3

System Requirements

To record this tutorial, I am using
  • Windows 11 OS and
  • FreeCAD version 0.21.2
Slide 4

Prerequisites

https://spoken-tutorial.org

To follow this tutorial,
  • Learners must be familiar with the FreeCAD interface.
  • For the prerequisite tutorials, please visit this site.
Slide 5

Part Design Workbench

Let us now learn about Part design workbench.

This workbench provides tools for creating 3 dimensional solid objects.

Using this workbench it is possible to design precise 3D mechanical parts.

Slide 6

Part Design Workbench

The Part design is intrinsically related to the sketcher workbench.

The sketcher workbench is used to create 2 dimensional geometries for use in Part design.

Open the FreeCAD.

Select File and New to open the new file.

Click on the Start dropdown.

Select the PartDesign workbench from the drop down.

Let us open FreeCAD.

I will open a new file.

I have selected the Part Design workbench.

In the Combo View under Tasks menus >> Select the Create Body. In the Tasks menu, under Start Part click on Create body.

A new Body needs to be created to draw a sketch.

Select the Create Sketch. Now under Start Body, click on Create sketch.

This creates a sketch view where you can draw the components.

Point to the planes(xy, yz,zx planes)

In the Combo View.

Point to the planes under Select feature.

On the panel we can see three planes in 3 mutually perpendicular directions.

In the Combo View under Select feature three planes are shown.

In the Combo view click XY-plane (base plane).

Click on OK.

Select XY-plane in the Combo View.

This denotes the top view.

Click the OK button to select the plane.

Shows the tool bars. Observe that new tools are shown on the toolbar.
Point to the x-axis.

Select Create line tool.

Now let us draw a vertical line from the x-axis.

Select the Create line tool from the tool bar.

Point to the x-axis.

Place the cursor on the x-axis.

Point to the Constrain point onto object symbol.

Point to the x-axis.

Place the cursor on the x-axis line.

You can see that the x-axis line changes to yellow.

You can see that a Constrain point onto object symbol appears near the cursor.

It denotes that the point is fixed to the line.

Left click on the line and drag the mouse vertically up.

Left click again.

Point to the constraint.

Left click to complete drawing the line.

Now click on the line to start drawing it.

Drag the mouse vertically upwards to draw a vertical line.

You can see a Vertical constrain symbol appearing near the cursor.

It represents the line drawn vertically.

Left click to complete the drawing of the line.

Point to the x-axis.

(point to the symbol while editing)

Now let us draw a horizontal line along the x-axis.

Make sure that the Create line tool is selected.

You can check that by seeing the symbol near the cursor.

Place the cursor on the line.

Point to Constrain point onto object symbol.

Place the cursor on the line.

You can see the Constraint Point onto object symbol near the cursor.

Click and drag the cursor horizontally to right side. Click and drag the cursor horizontally to draw a horizontal line.

Now you can see two symbols appearing near the cursor.

Constrain point onto object symbol and Constrain horizontal symbol.

Left click on the line.

Select the constrain.

Click to see the red line.

We don’t want two Constraint point onto objects.

This means that the line is fixed at two points to the same object.

Upon clicking, you can see that the entire drawing has turned to red.

Click on any one of the constraints.

Press the Delete key on the keyboard.

To clear that, click on any one of the constraints.

Press the Delete key on your keyboard to delete the constrain.

point to the drawing. Now you can see that the drawing came back to normal.
Select Create line tool.

Place the cursor on the x-axis and click and drag the cursor.

Place the cursor slightly lower than the x-axis and left click.

Let us avoid the appearance of the Constrain Point Onto Object symbol twice.

To do this, let’s draw a line below the x-axis.

Right click the mouse button.

Press Esc key.

To deselect the tools, right-click on the panel.

Or press the Escape key to deselect the tools.

Cursor on the interface. Now let us draw an arc.
Select Create arc tool.

Place the cursor at the top of the vertical line.

Select the Create arc tool from the tool bar.

Place the cursor on the top end of the vertical line.

You can see that a X-Shaped symbol appears near the cursor.

It is the Constrain coincidence.

It denotes that the cursor is at the top of the end point.

Left Click and drag the cursor outside.

Left click and drag the cursor to the left.

Drag the cursor to draw.

Left click on the mouse.

Now left click and drag the cursor to left or right.

You can see a model circle that can be drawn.

Click to release the model circle.

Drag the cursor to start drawing the arc.

Left click again to finish the arc.

Select Create circle tool.

Place the cursor on the end of the horizontal line.

Left click and drag the cursor.

Left click again.

Left click to finish the circle.

Now let us draw a circle.

Select the Create circle tool.

Place the cursor at the end of the horizontal line.

Check for the X-Symbol.

Left click and drag the cursor to draw the circle.

Once the definite size is visible, left click to finish the circle.

point to the objects. Observe that, we have drawn these shapes with no dimensions.

Let us assign some values to them.

Select the vertical line.

Select Constrain vertical distance tool.

Fill the Length field as 30 mm.

Let us select the vertical line.

Select the Constrain vertical distance tool from the tool bar.

Insert length pop up appears.

In the Length field type 30 mm and click the OK button.

Point to the line. You can see that a dimension is applied to that line.
Select the horizontal line.

Select Constrain horizontal distance tool.

Fill the Length field as 30 mm.

Now select the horizontal line and click the Constrain horizontal distance tool.

Insert length pop up appears.

In the Length field type 30 millimetre and click the OK button.

Select the arc.

Select the arrow near the Constrain arc or circle tool.

In the drop down select Constrain radius.

Fill the Radius field as 10 mm.

Now to set the radius of the arc, select the arc.

Select the arrow near the Constrain arc or circle tool.

In the drop down select Constrain radius.

Insert radius pop up appears.

In the Radius field type 10 mm and click OK.

point to the circle. Now let us give the dimensions to the circle.
Select the Circle.

Select the arrow near the Constrain arc or circle tool.

In the drop down select Constrain radius.

To set the radius for the circle, select the circle.

Select Constrain radius.

Fill the Radius field as 20mm

Click OK.

Insert radius pop up appears.

In the Radius field type 20 mm and click OK.

In the Combo View click on the Close button. In the Combo View click on the Close button to complete the sketch
Slide 7

Industrial Drawing

modeldrawing.png

Now let us use the tools to draw a Flange coupling.
Select New file. Now I will open a new file.
Select Create body.

Click Create sketch.

Select XY-plane (base plane) in the Combo View.

Click on OK.

We can select the Create body tool from the toolbar.

Then select Create sketch.

Select XY-plane and click OK.

Select the Circle tool.

Place the cursor in the horizontal line on the left side.

Now let us draw two circles.

Select the Create circle tool and place the cursor on the x-axis.

You can see that line changes to yellow color.

You can see that Constrain point onto object symbol appears near the cursor.

Click the line. Now click on the line to draw a circle.
Draw another circle on the right side on the same line. Repeat the process on the other side of the x axis.
Right click to deselect the tool. Now right click the mouse to deselect the tool.
Select the center of the left side circle and midpoint of the plane.

Select Constrain Horizontal Distance tool.

Select the center of any one of the circles and the midpoint of the plane.

Once the points are selected they turn to green color.

Click Constrain Horizontal Distance tool.

In the length field type 100 in the dialog box.

Click OK.

In the Insert length dialog box, type the length as 100 millimetre and click

OK.

Select the centers of both the circles.

Select Constrain Horizontal Distance tool.

In the length field type 200 in the dialog box.

Click OK.

Select the centers of both the circles and click Constrain Horizontal Distance tool.

Change the length to 200 mm.

Click and hold the middle mouse button and move the mouse.

(look for the four sided- move cursor)

Let us move the drawing to a convenient place to see it clearly.

Press and hold the middle mouse button to see the move cursor.

Move the mouse and place the drawing at a convenient location.

Select Create arc tool. Now select the Create arc tool.
Place the cursor on the center of the left circle. Place the cursor on the center of the circle.

You can see that midpoint changes to yellow color.

An X-shaped symbol appears near the cursor.

This denotes that the cursor is at the midpoint of the circle.

Click the midpoint and draw a semi-circle from bottom to top.

Semi-circle should be on the left of the circle

Now click on the midpoint and draw a semicircle from bottom to up.
Click the midpoint of the right side circle and draw a semicircle.

Semi-circle should be on the right of the circle.

Repeat the same process on the other side.
Click the midpoint of the plane.

>> draw one arc at the top and another at the bottom.

Let’s draw two more arcs above and below the plane from center of the plane.
Select the line tool.

Join all the arcs one by one.

Now, select the Line tool and connect all the arcs.

Make sure to click only when the X-symbol is visible.

Select the top left line and the top arc.

Select the Constrain Tangent tool.

Now select a line and the arc and select the Constraint Tangent tool.

This makes the connection between the arc and line smooth .

Select a line and the arcs.

Select the Constraint Tangent tool.

Repeat this process for the arcs and lines at four points to make them smoother.
Select the top arc.

Click the arrow near the Constrain arc tool.

Click Constrain radius tool.

In the radius field type 75 in the dialog box.

Click on OK.

Now select the top arc and click Constraint radius tool


Set the radius to 75 mm.

Click Constrain radius tool.

In the radius field type 75 in the dialog box.

Click on OK.

Let us change the radius for the bottom arc also.
Select both the circles.

Click Constrain radius tool.

In the radius field type 10 in the dialog box.

Click on OK.

Now select both the circles and click Constraint radius tool.

Change the radius to 10 mm.

Select both the arcs around the circle.(left and right)

Click Constrain radius tool.

In the radius field type 30 in the dialog box.

Click on OK.

Select the arcs around the circles and change the radius to 30 mm.
Click Close in the Combo view. Click Close in the Combo view.

You will exit the sketch view

Select top in the Gizmo. Now select the Top view from the Gizmo.
Select Pad tool. Select the Pad tool from the tool bar.
point to the sketch You can see that the sketch will turn into a 3D object.
In the length field type 20 in the dialog box.

Click on OK.

In the Combo view change the length to 20 mm.

This will increase the thickness of the drawing making it 3 dimensional.

Then click the OK button.

Press and hold both the middle mouse button >> right click and move the mouse. Let us rotate the drawing.

Press and hold the middle mouse button.

Right click and move the mouse.

Or you can change the view using the gizmo.

Click Create sketch.

Select XY-plane (base plane)

Click on OK.

Again click Create sketch.

Then click XY-plane.

Click the OK button.

Select the View section tool. Select the View section tool to clearly see all the points.
Draw a circle from the center of the plane.

Select the circle.

Click on Constrain radius tool.

In the radius field type 50 and click OK.

Now draw a circle from the center of the plane.

Set the radius to 50 mm.

Click the Close button.

Select Model tab. Go to the Model tab in the Combo view.
Select the sketch. Select the sketch if not already selected.
Select Pocket tool.

In the Combo view, type 20 in the length field.

Check the Reversed check box.

Click on OK button.

Now select the Pocket tool from the tool bar.

Pocket tool is used to create holes in already existing drawings.

In the Combo view, change the length to 20 mm.

Tick the Reversed check box.

Click the OK button.

Change the view to front. Now change the view to front using the gizmo or from the tool bar.
Point to the 3D component. The 3D component is ready.
Click File and Save.

Enter a Name and click Save.

Now let us Save the file with an appropriate name.
Only Narration. With this we come to the end of this tutorial.

Let us summarize.

Slide 8

Summary

In this tutorial, we have learnt to,
  • Draw basic shapes.
  • Use basic constrains.
  • Draw the Flange Coupling component in 3D.
Slide 9

Assignment

For the assignment activity, please do the following:
  • Practice to draw different shapes.
  • Practice pad and pocket tool.
Slide 10

About spoken tutorial project

This video summarizes the spoken tutorial project.

Please download and watch it.

Slide 11

Spoken tutorial workshops

We conduct workshops using spoken tutorials and give certificates.

Please write to us.

Slide 12

Forum

Please post your timed queries in this forum.
Slide 13

Acknowledgement

Spoken tutorial project was established by the ministry of education government of India.
Slide 14

Thank you

This tutorial is contributed by Dr. Sathiya Narayanan and K.Sakthivel.

Thank you for joining.

Contributors and Content Editors

Madhurig

Retrieved from "https://script.spoken-tutorial.org/index.php?title=FreeCAD/C3/Introduction-to-Part-Design-Workbench/English&oldid=56629"