Basic Part Design Tutorial 019

From FreeCAD Documentation
Revision as of 00:30, 11 November 2022 by Edwilliams16 (talk | contribs) (→‎Sketch002: Switched 5 and 11 dimensions.)
This documentation is a work in progress. Please don't mark it as translatable since it will change in the next hours and days.
Tutorial
Topic
Modeling
Level
Beginner
Time to complete
Less than an hour
Authors
Carlo Dormeletti (onekk)
FreeCAD version
0.19 or higher
Example files
[]
See also
None

This tutorial introduces the new user to some of the tools and techniques used in the PartDesign Workbench. This tutorial is not a complete and comprehensive guide to the Part Design Workbench and many of the tools and capabilities are not covered. This tutorial will take user through the steps needed to model the part shown in the image below using sketches.

Author Note: This tutorial is work in progress, in this state it is tested only with FreeCAD version 0.20.1 for Linux. Screenshots are made for 0.20.1 too, but it should work without big problems even on 0.19.

As soon I find someone to review it for 0.19 I will made appropriate remarks if necessary for v0.19


Before You Begin

The Task

In this tutorial, you will be using the Part Design Workbench to create a 3D solid model of the part shown in the Drawing below. All of the necessary dimensions to complete this task are given. You will start by creating a core shape from a base Sketch and then build on that shape, adding what is known as Features. These features will either add material to, or remove material from the solid by use of additional sketches and accompanying feature operations. This Tutorial will not use every feature and tool available within the Part Design Workbench, but should use enough to give the user of this tutorial a basic foundation upon which to build their knowledge and skills.

The Part

Constructing The Part

Startup

First begin by making sure you are in PartDesign Workbench. Once there, you will want to create a new document if you have not done so already. It is a good habit to save your work often, so first save the new document, giving it any name you might like.

All work in Part Design begins with a Body. Then we will build the solid inside the body by starting with a sketch.

Click on Create new body to create and activate a new Body Container. Note: this step can be omitted. When creating a sketch using Part Design|Sketch|Create Sketch, if no existing Body is found, a new one is automatically created and activated. This is not the case if you create a sketch using the Sketcher workbench, as sketches are useful in workbenches other than Part Design.

Master Sketch

You will create a master sketch, see maybe Sketcher WorkBench for a more detailed explanation of the terminology used here.

The workflow follows one of the many possible ways to make the above design.

This example will use some techniques described in Advice for creating stable models.

  1. master sketch
  2. Named constraints are used to hold dimensions that can be readily referenced later in the model construction.
    For instance, to change the model width from 53 mm, as in the technical drawing, to 55 mm we need only to modify the Length value of the appropriate named constraint in the master sketch and the whole model will modify accordingly. This is parametric design in action.
  3. External Geometries that could be subject to Topological Naming Problem, will be used only when strictly necessary and trying to refer stable elements.

Rationale

  1. The Master sketch contains the model's rectangular base shape and two named constraints that will be used to supply correct dimensions to other parts of the model:
  2. length that will contain 53mm. (The result of adding the 39mm dimension to the two 7mm "sides")
  3. width that will contain 26mm.

Caveats:

  1. If you had checked Auto constraints in Edit controls window, some constraints will be applied automatically, if not:
    Make sure that you have exited the Polyline tool by right-clicking or pressing ESC twice; the mouse cursor should turn back from a cross-hair to the standard arrow cursor. (Don't press ESC a third time or you will exit the sketch editing mode; if this happens, click on the Model tab, then double-click the Sketch element in the tree, or right-click and select Edit sketch in the contextual menu.)
  2. If Sketcher's Solver detects a redundant constraint it will turn the sketch orange in color. Before further constraints are added, redundant constraints should be removed. (Redundant constraint are shown in the Task view, click on the blue reference and press DEL.)
  3. It's possible that some elements of the side panel, as example OK button may not be visible if the side panel is not wide enough.
    You can make it wider by dragging its right border.
    Place your mouse pointer over the border; when the pointer changes to a two-way arrow, press and hold the left mouse button and drag.
Fig: SK1
Fig: SK2

Sketch

  1. Click on Create new sketch. This will create the sketch within the just created body. It will be named Sketch.
  2. A dialog like Fig: SK1 will open in Tasks tab on which you have to choose on which plane sketch will be attached.
    1. Select XY_Plane in from the Combo view list.
    2. Press OK
  3. FreeCAD automatically:
    1. switches to Sketcher workbench
    2. opens the sketch in editing mode and you will see something like Fig: SK2.


Rectangle creation

Fig: SKC1
Fig: SKC2
Fig: SKC3
Fig: SKC4

Click on Rectangle tool and start creating a rectangle this way:

  1. Create the rectangle roughly centered on Y axis something that resemble Fig: SKC1. Note:
    1. Don't place points X axis as the Solver will automatically apply constraints that will create some problem later.
    2. It is not important at this step to state exact dimensions, exact dimensions will be assigned using constraints in a later step.
  2. Once done press ESC to exit "rectangle creation mode". "Rectangle creation mode" is indicated by this cursor appearance .


Horizontal constraint

Assign now horizontal distance constraint this way:

  1. Select line defined by P2 to P3 in Fig: SKC1.
  2. Use button horizontal distance constraint this will make two things:
    1. A dimension will appear between extreme points of the line selected. This dimension is the actual dimension.
    2. Additionally a dialog will appear:
      dimension dialog
  3. Assign a Length = 53mm, and to be able to reference the dimension later a name is required as well: assign Name = length.
  4. Click OK.
  5. The result should resemble Fig: SKC2


Symmetrical constraint

To center the the top edge of the rectangle around the origin proceed as follows:

  1. Select points P2 and P3 of the rectangle.
  2. Select the origin of the sketch.
    Note: selection order of the points is important.'
  3. Using Symmetric tool.
  4. You will end up with something that resembles Fig: SKC3.
  5. Making a good choice of origin of the model can simplify its construction, in this case by taking advantage of the part's reflection symmetry in a later steps.


Vertical constraint

You now assign a vertical distance constraint, the procedure is similar to that for the horizontal distance constraint

  1. Select line defined by P3 to P4 in Fig: SKC1.
  2. Click on vertical distance constraint and assign:
    1. Length = 26 mm
    2. Name = width.
  3. Click OK.
  4. Result must resemble Fig: SKC4.

Note a couple of things:

  1. Lines on the sketch will become "bright green". (Assuming you have not modified the default color theme).
  2. Solver messages window displays Fully constrained.
  3. If you click on a line or vertex and try to drag it, it won't move.

Side Profile

You will create a new sketch that is holding the side profile.

Sketch001

File:Pd tut sp01.png
Fig: SP1
  1. Click on Create new sketch. This will create the sketch within the just created body, and FreeCAD will assign the name of Sketch001.
    1. When choosing the plane you will select YZ_Plane in the list and press OK:
  2. Use the Polyline tool and make a shape roughly like that in Fig: SP1;
    1. Follow the order of point indicated in the image (It is not obtained using FreeCAD, but mimics decently the real appearance with default color theme).
    2. Exact shape is not important as like in the first sketch you will assign proper constraints later (see note about Constraints below).


Constraints

Fig: SPFC

From Fig: SP1 you will see that FreeCAD has already applied some constraints:

  1. Top horizontal line has a Horizontal Constraint applied.
  2. Right point of the top line has a Point On Object Constraint applied.
  3. Left point of bottom horizontal line has another Point On Object Constraint applied.

Note: It may be easier for a less-experienced user of Sketcher to make the initial drawing offset from the axes and then apply the constraints "by hand". For instance, just because two points look coincident, doesn't mean they are. Any constraint has to be explicit. When selecting vertices or lines with sketcher tools they will turn (default) green and any auto-constraints that will be applied will show beside the cursor.

  1. Select line defined by points P2 and P3 and apply a horizontal distance constraint and assign Length = 5 mm.
  2. Select line defined by points P1 and P2 and apply a vertical distance constraint and assign Length = 26 mm.
  3. Select line defined by points P4 and P1 and apply a horizontal distance constraint for the value you will use a "Named constraints" using Expressions to do so you have to press the little button on the dimensions , and you are presented with a new dialog window named Formula editor that contains an input field and a Result: label, similar to the image below:
    Expression dialog
    Expression dialog

    if you start typing in the cell, you will be presented with some autocompletions, base on the "Name" of the sketch, in the example is <<Sketch>>.
    1. Select the right one for your design; Field should have autocompletion so when an element is selected you will be presented with <<Sketch>>., note the point after the "element name".
    2. To select named constraint "width", you have to write the word Constraints. with the point, here autocomplete will work.
    3. To add "length" sadly you have not yet autocomplete, so complete the cell to read <<Sketch>>.Constraints.width if all is good you should see in the cell Result: the correct value as in figure below:
      Espression result good
      Espression result good

      Note the absence of "red words" and the correct value in the Result field
    4. Click OK to close Formula editor dialog.
    5. Click OK to close Insert length dialog.


Finalizing the Sketch

At this point you should have a fully constrained sketch as indicated by it changing color and the message shown in the Combo View. It should now look just like Fig: SPFC:


Note the differences in color between distance constraints assigned using expressions and those assigned specifying a length.


Now in the Tasks tab, click on the Close button to leave the sketch edit mode

Pad

Fig: Pad

Select Pad from the toolbar or from the Part Design menu.


This will give you a Pad dialog in the Task View.

Using that dialog, set it's values accordingly to the following directions:

  1. For Type select Dimension .
  2. For Length you will use again an Expression but this time you will enter <<Sketch>>.Constraints.length in the field.
  3. Select Symmetric to plane.

Once that is done you will have a solid as shown in Fig: Pad


Features

Fig: SK2
File:Pd tut sk2 ext geom.png
Fig: SK2_1
Fig: SK2_2
Fig: SK2_3

With Pad you have obtained a solid.

Now it is time to add some Features to this solid..

These Features could be obtained in various way, the way presented here is not the only way to achieve desired result.

Starting point is another time a Sketch.

Sketch002

  1. Hide the just created solid selecting it and using Spacebar to hide, or using the
  2. Click on Create new sketch in XZ_Plane; Sketch will be named Sketch002.
  3. Select Rectangle tool, and create a rectangle, do not create it using near the axis, to avoid automatic constraints that will make difficult to move it in the correct position using External geometry tool.

    Apply these constraints:
    1. Select one of the horizontal lines apply a horizontal distance constraint and a value of 11 mm.
    2. Select one of the vertical lines and give it a vertical distance constraint and a value of 5 mm.
      You should obtain something similar to Fig: SK2.
  4. Click Close at top of the Tasks tab in the Combo View window.


External geometries constraints

To use an External geometry is necessary to have sketches on which we are "attaching" our geometry visible.

  1. In the Treeview select Sketch and Sketch001 and make both visible using Spacebar.

With Sketch and Sketch001 visible, it is easy to operate:

  1. Double click on Sketch002 to activate again edit mode and adjust the view so you have clearly visible the points as example like in Fig: SK2_1, this will ease subsequent steps.
    Note: position of the rectangle could be different on your draw.
  2. Select External geometry tool, the cursor will became .
  3. Select with this cursor point P1 in Fig: SK2_2, selected point will remain highlighted and in the Elements tab of Task Panel you will see that this element is shown File:Pd tut ext geom pt.png.
  4. Select with this cursor point P2 in Fig: SK2_2.
    In the Elements tab of Task Panel you will see another element like the above.
  5. Press ESC to terminate External Geometry selection. Cursor will return standard arrow pointer.
  6. Select point P1 and point P3 and apply a Vertical Constraint.
    Rectangle will be aligned with the vertical position of selected point.
  7. Select point P2 and point P3 and apply a Horizontal Constraint.
    Rectangle will be aligned with the horizontal position the selected point.
  1. Click Close button at top of the Tasks tab in the Combo View window.


Pockets

Fig: PK1
Fig: PK2

You have to subtract some material using the just created sketch that is positioned at one end. To make this operation you have to use Pocket tool from the toolbar or Part Design menu.

Using this tool is the opposite of the Pad tool. As the Pad tool adds material to the part, the Pocket tool removes material from the part.

Pocket

  1. Select Pad and Unhide it.
  2. Select Sketch002.
  3. Select Pocket and configure the operation:
    1. Select Type Through all .
    2. Check Reversed
    3. Click the OK button.

You should have something that resemble Fig: PK1

Mirror

Instead of creating another sketch and pocket it, as the model is created using the Y axis as a symmetry axis, you could easily duplicate the pocket using Mirrored.

  1. Select “Pocket”.
  2. Click on the Mirrored feature on the toolbar or from the Part Design menu.
    A dialog will appear in the Combo View.
    1. Select Plane Vertical sketch axis from the pulldown menu.
    2. Click OK
      If all has gone well, you should now have a part that looks like Fig: PK2

Sides

Sketch003
Fig: Pad001
Fig: Mirrored001
  1. Make Sketch visible as done in precedence.
  2. Click on Create new sketch in XY_Plane; Sketch will be named Sketch003.
  3. Select Rectangle tool, and create a rectangle.

    Apply these constraints:
    1. Select one of the horizontal lines apply a horizontal distance constraint and a value of 7 mm.
    2. Select one of the vertical lines and give it a vertical distance constraint using an Espression and assign a <<Sketch>>.Constraints.width.
    3. Add an External geometry using the point P1 as shown in Fig: SK2_2
  4. Click Close at top of the Tasks tab in the Combo View window.
Pad001
  1. Select Sketch003.
  2. Click Pad and assign these values:
    1. Type = Length .
    2. Length = 16,70 mm
  3. Click Close at top of the Tasks tab in the Combo View window.
    You should have a result as shown in Fig: Pad001
Mirrored001
  1. Select “Pad001”.
  2. Click on Mirrored and assign:
    1. Select Plane Vertical sketch axis from the pulldown menu. (It should be already selected, but check)
  3. Click OK
    If all has gone well, you should now have a part that looks like Fig: Mirrored001

Center Hole

File:Pd tut cp01.png
Fig: CP01
File:Pd tut cp02.png
Fig: CP02

Now it is time of the most challenging thing, in the design above, you will easily see that central pocket dimensions are referred to the slanted face.

This will surely lead to Topological_naming_problem as you could refer to the face that is created using Sketch001, a different solution is to use Sketch001 to model another sketch as follows.

Sketch004

  1. Make Sketch visible as done in precedence.
  2. Click on the New sketch icon in the toolbar or from the Part Design menu. This will create a sketch named Sketch004.
    1. Select YZ Plane
  3. Using Polyline tool, trace a polyline like those indicate with points P1, P2, P3, P4 in Fig: CP01.
    Note:
    1. Trace polyline slightly over X axis.
    2. Remember to close polyline clicking first point as last point, this will correctly make the coincident constraints.
    3. Note applied constraints, if they are not applied using Auto constraints apply manually:
      1. Constraint horizontal on lines defined by P1 to P4, and P2 to P3.
      2. Point on object on P1 and P2 on the Y axis.
  4. Using External geometry tool select line defined by EGP1 and EGP2 on Sketch001 indicated in Fig: CP02 with purple color.
  5. Apply Point on object to P3 and P4, selecting the point and the external geometry, this will make line P3 to P4 coincident with line defined by EGP1 and EGP2 in Sketch001.
  6. Apply Distance to line P3 to P4 and assign Length = 17.00mm
  7. Apply Distance to P4 and EGP2 and assign Length = 7.00mm
    This will result in a fully constrained sketch like in Fig: CP02.
  8. Close Sketch004

Pocket001

Now it is time to make the central pocket, remember that the central pocket has to respect some distance to the side pad marked as 11mm distance, but with some easy calculations it will became evident that the pocket is simply centered on the face, this will ease the pocket positioning.

  1. Select Sketch004.
  2. Select Pocket and configure the operation:
    1. Select Type TwoLengths .
    2. Assign 8,50mm to Length and Length2 values
    3. Click the OK button.
  3. Select the newly created Pocket001 and modify Refine property to True

This will result in:

This tutorial and your model are complete.

Additional Resources

File to make comparison with your results: