Engineering Homework (CAD Program Using)

Solid Modeling Assignment

EGR 201-100

Spring 2018

Extra Credit Value: Equal to 2 homework assignments or in-class quizzes.

Due Date: March 19th by Midnight.

Assignment:

1) Using CAD (computer aided design) software, reproduce the four technical drawings.

2) Complete the survey.

3) Submit documents by email to [email protected]

Note: if you have access to Solidworks or another program and wish to use it instead, then produce the

four technical drawings and turn them in for full credit. You don’t have to use FreeCAD.

Note: the survey is part of the grade, so make sure you fill it out.

Table of Contents

Purpose of this Assignment .................................................................................................... 2

Background on Solid Modeling ............................................................................................... 2

Software Installation ............................................................................................................. 3

Assignment ........................................................................................................................... 4

Survey ................................................................................................................................... 8

Tutorial and Creating Part 1 ................................................................................................... 9 Step One - Base ............................................................................................................................ 10 Step Two – Top Notches ............................................................................................................... 14 Step Three - Extrusion .................................................................................................................. 17 Step Four – Center Hole ................................................................................................................ 18 Remove Duplicated Volumes ........................................................................................................ 20 Produce Technical Drawing ........................................................................................................... 20

Purpose of this Assignment By drawing 3D models and producing technical drawings, you will learn to interpret x,y,z coordinates on

engineering drawings, such as those found in the Engineering Statics textbook.

Background on Solid Modeling CAD software generally fit into one of two categories:

Solid modeling - modeling solid shapes (volumes). Materials are clearly defined.

Surface modeling - modeling wireframes and surfaces, which are hollow.

Solid modeling is clearly useful if we want to investigate stresses and strains in our designs. You

can draw solid volumes, assign material properties (wood, brick, steel, glass, aluminum), and then

subject them to loads. Generally, most engineering professions use solid modeling. 3D animators,

architects, and video game designers use surface modeling.

The method for solid modeling is to start with a general solid outline of the shape, and then

make several cuts and extrusions to make it into the final part. Note that this is fundamentally different

than how models are created using wireframe/surface modeling software. If you want to try that

different kind of modeling, both Blender and Sketchup are free. Another fundamental difference is that

in solid modeling, everything is in reference to a prior operation (cut, extrusion). You will see a

hierarchical list of operations in the left hand panel, and changing something high on the list will cascade

changes down the list. In surface modeling, the entire model is just a list of vertices and lines – or a list

of triangles. Changing one part does not affect the rest.

These software titles are marketed to profitable engineering companies and animation studios,

so licenses can be $4,000-$50,000 per user per year. However, as a student there are ways to get many

of them for free or use free alternatives.

A typical workflow for solid modeling is the following: 1) Parts – make individual parts. 2)

Assembly – assemble parts together to make more complicated objects. 3) Finite element method (FEM)

– solve how the structure will deform when subject to assigned loads. This is done by creating meshes of

points and solving massive matrices of differential equations. This is covered in a Mechanics of Materials

course.

Examples of Solid Modeling Software

Solidworks

Ansys

Creo (formerly Pro-E)

Coventerware

Rhinoceros 3D

FreeCAD

Examples of Surface Modeling Software

Maya

3DS Max

Blender

AutoCAD

SketchUp

Cinema

Software Installation The tutorial below assumes use of FreeCAD 1.6 with the Drawings Dimensioning add-in. It is also

possible to complete this assignment with FreeCAD 1.7, using the built-in Technical Drawings tool, but

you will have to find a tutorial for that online. Also, you can use commercial software such as Solidworks

if you have access.

The main software (Windows, Mac, Linux) is available to download and straightforward to install:

https://www.freecadweb.org/wiki/Download

On OSX, the first time you open it you will have to right click (ctrl click) and choose Open. This is to

confirm you trust the software.

To produce engineering drawings, we will also need these additional tools:

https://github.com/hamish2014/FreeCAD_drawing_dimensioning

To install this tool: download, unzip, and place the entire folder into…

Windows: C:\User-Name\Appdata\Roaming\FreeCAD\Mod\ (replace User-Name with your user name)

OSX: Place the unzipped downloaded folder into /Applications/FreeCAD.app/Contents/Mod/

Then, restart FreeCAD.

Finally, we need a vector graphics program so we can write our names on the engineering drawings we

produce. Inkscape is free (if you have Adobe Illustrator, that works too).

https://inkscape.org/en/

Note that if you use the OSX version of Inkscape, shortcuts use ctrl like in Windows and not the Apple

key (⌘).

Assignment Draw the following parts using solid modeling software and reproduce the technical drawings. The

drawings must be fully dimensioned and include a label with your name, the date, and the title (Part 1-

4). The technical drawings must include at minimum the following views: front, side, top, and isometric.

The “front” direction should match that in the given drawings.

There are four drawings in total.

Survey Complete this survey and turn it in along with your drawings.

1. Have you used CAD software before?

2. How long did it take you to complete the tutorial (write N/A if you didn’t use it)?

3. How long did it take you to complete the remaining three drawings?

4. Did drawing these 3D models aid you in understanding the technical drawings in the book (see

examples below)?

5. Do you value that you learned introductory CAD?

Tutorial and Creating Part 1 This tutorial has been adapted from https://www.freecadweb.org/wiki/Basic_Part_Design_Tutorial

The FreeCAD interface is shown below. At any time, you will see a subset of the available tools in the

toolbar, depending on what is selected in the “Workbench Selector.” Noted in the figure are view

options and the model navigator. The model navigator has two uses: it lists the operations in order and

shows tool options when you’re using a tool. The model navigator is hierarchical, so changing an

operation high up on the list will cascade those changes down the list.

This tutorial will teach you to draw this part and produce a technical drawing of the part. We will use all

of the standard tools, such as cuts and extrusions.

Left: The result of this tutorial – a technical drawing. Right: An alternative technical drawing.

Step One - Base

Press New Document (top left corner)

Expand the Workbench Selector menu – Choose Part Design (top middle)

Now your toolbar should look like this.

It is a good habit to save your work often, so before anything else save the new document, giving it any

name you might like.

Press the New Sketch button. We will draw a 2D profile first that we will modify. For the options, choose the y-z plane. The view will automatically rotate to see the y-z plane.

The Polyline tool lets you draw shapes – click once for each vertex. Draw a sketch similar to the right. It doesn’t need to be exact – we will make it exact in the next step by defining the exact lengths and whether lines are vertical or horizontal. When first drawn, it will be gray. Once fully defined, it will turn green like in the sketch to the right. Press ESC to exit out of the poly tool.

Now we will fix up the drawing to be exact. Perform selections of sides or points and then assigning

constraints. Select multiple by clicking in succession or by dragging a box. The constraints are in the

bottom red toolbar:

Select the two horizontal lines with your mouse by clicking on them, and once selected, click on

the horizontal constraint.

Select the vertical line on the right and then click on the constraint.

Select the start and end points of your polyline and click on the coincident constraint to close the

polyline. You can select points that are near each other by drawing a box.

Select the bottom horizontal line and the right vertical line and apply an Equal Length constraint.

Select either the long horizontal or vertical line and apply either a vertical length

constraint or horizontal length constraint of 26 mm.

Select the top horizontal line and apply the horizontal distance constraint and give it a value of 5

mm

Select, in this order, the lowest left point, the upper right point, and then the origin (see

diagram). You can select by just clicking them in order, you don’t need to hold shift or ctrl. Then press

the symmetry constraint.

Now your drawing should be fully defined, and should turn green to indicate this.

Exit the sketch drawing mode by pressing Close in the Combo View dialogue box.

1

3

2

Now, with the Sketch 1 in the Navigator highlighted, press Pad to give a depth to the sketch. The total length should be 53 mm, but we would like it centered on the y-z plane. This can be done by choosing “Two Dimensions” and setting them both to 26.5 mm. Note that in FreeCAD, an extrusion is called a “Pad” and a cut is called a “Pocket.”

Now your model is 3D! But how to view it from different angles? First there are the view buttons if you

want to see axiometric view (45 deg looking down) or a specific plane.

If you ever get into a weird view and want to reset, press the left button

(axiometric) and fit content on screen.

If you want to see from an arbitrary view, right click anywhere and choose a navigation style. I think Gesture is the most intuitive and simple – left click and drag to rotate, right click and drag to pan. Mouse wheel to zoom. The options are summarized below. Try viewing your part from all angles. When ready, finish drawing the part by modifying the shape we have already.

Step Two – Top Notches First, rotate the sketch so that you can see the back, and select it.

Next, press the New Sketch button. A new sketch will be created which is on the same plane as the back face. The view should rotate so that you can see the sketch.

This time we will draw with the rectangle tool. Make a rectangle like the following. It doesn’t have to be exact, we will dimension it like last time. PRESS ESC TO EXIT THE RECTANGLE TOOL. Pressing ESC twice will exit the sketch, which you don’t want to do.

If you accidentally exit the sketch, double click on the part browser to re-enter the sketch. Or right click the sketch in the browser and choose “edit.”

In the sketch, select the appropriate sides and:

Set the width to 5 mm.

Set the height to 11 mm

This tool, External Geometry, adds a reference point in our sketch to outside geometry. Add a

geometry reference to the upper right part of the face we are working on. If the button is not visible

(likely if your screen resolution is less than 1080p), it may be hidden behind a >> arrow, as below.

Now use this tool, the “Coincident” tool, to lock the rectangle we drew to the external reference point. The result should be as in the diagram to the right.

Now we will use this sketch to make a cut, which is with the Pocket tool. Exit the sketch by pressing Close in the Combo View or by pressing ESC a bunch.

Press the Pocket button. Notice that you can make a cut to a specified depth, but we will choose “Through” to go fully through the part.

Click ok and rotate your part around – you can see the cut we just made. If you go back to the original drawing, you’ll see we need to make a similar cut on the other side. We could do it the same way, with a new sketch, or even by adding another rectangle to the sketch we just drew. However, an alternative is to use the mirror button.

Select the Pocket we just made in the model tree, and then press this mirror button. Now you see why we drew the part by extruding +/-26.5 mm, so that we can mirror easily. Otherwise we would have had to draw an additional reference plane to be the mirror. Choose horizontal mirror and press ok.

The result:

Remember to save periodically.

Step Three - Extrusion

Next, make a new sketch on the same back plane as before. Select the back plane and press

Sketch.

Same as last time, draw a rectangle, dimension it, and link it to the corner using an external geometry reference. The result should be like this, highlighted in green meaning that it is fully constrained. Exit the sketch by pressing Close in the Combo View or pressing ESC a bunch.

This time we will use the Pad tool to make an extrusion. Set the extrusion to 26 mm. You may have to click “Reversed” or type in “-26 mm” in order for it to go the correct way. If it is backwards, double click on the part in the Model list to edit. The result should be like the right.

Mirror again. Click on the new Pad0001 and click Mirror. Horizontal axis. Press OK.

Step Four – Center Hole For the next step, we will cut the center hole, the last step in creating the model. From the given design,

we know that it is a hole that goes straight back and makes a 17 mm square on the front face. If we

draw the square on the front face and try and extrude (Pocket), then you will find the software is limited

in making a cut perpendicular to the face, which is not the direction we want. There are several ways to

get around this, such as making a reference plane to draw the sketch on or cutting from the back face

forward. We will do the second one. In order to know the shape of the 17 mm square when projected

onto the back face, we could calculate it based on the angle of the front face. it is easier to use a

reference from the front face. First create the front face reference square.

Select the sloped face to become the plane for our next sketch and make a new sketch.

Make a rectangle in the center.

Make it constrained to a square by clicking on a horizontal side and vertical side and making them equal in length.

Make the side length 17 mm using either of these two tools.

Make an external reference point to the point on the upper right of the sketch area (see diagram)

Select both the upper right corner of the square and the external reference point, and set the distances to 7 mm horizontal offset and 11 mm vertical offset. The square should turn green, meaning it is fully defined. Now exit the sketch by pressing ESC a lot or pressing Close.

Turn the sketch into a 1 mm pad. This is so we can use it as a reference point, since you can only

reference features.

Start a new sketch on the back face.

Before doing anything, rotate the view so that you can see the front face. Then press the External Reference button and add two of the sides of the square as a reference. Note: when in Sketch edit mode and using Gesture navigation mode on OSX, you cannot rotate with left click as usual. If you hold alt and then click and drag, it should rotate.

Either navigate to see the back face again or press this button to automatically show the back (shortcut is the 4 key). Now your sketch should have two reference edges to use, which are the projection of the 17 mm square onto the back face.

Make a rectangle and snap it to the reference geometry.

If you didn’t snap it when creating the rectangle, you can use the Coincident Constraint tool to snap the rectangle, after drawing the rectangle. When complete, the rectangle should be green, showing that it is fully defined.

Now exit the sketch and use the pocket tool to go Through All. Notice that the other pad, which uses the same geometry, is erased. The completed part is shown to the right. Save the model.

Remove Duplicated Volumes Before proceeding, I recommend doing Save-As with a new title. You will have two document versions: the completed part, and a second version which includes the Refine Shape and Drawing you will produce in the next steps. Show the OpenSCAD toolbars. OpenSCAD is actually another software tool for editing CAD files, and has been added to FreeCAD.

Highlight your last Pocket you made in the combo view.

Press the Refine Shape tool. It will remove duplicated volumes, and the resulting part should look cleaner, like the below.

Produce Technical Drawing In the next version update, 1.7, FreeCAD has a much better tool for producing technical drawings called

TechDraw. However, it is very buggy. Instead we will use an extension of the tool in version 1.6, called

Drawing Dimensioning. This is also buggy, so I just want you to produce minimum technical drawings

which you will turn in.

Installation instructions for Drawing Dimensioning are above, in the software section. With your model open, go to the Drawing Dimensioning workbench.

Create a new page, and choose A4 Landscape (ISO7200). We are choosing A4 instead of letter because the letter format is buggy. Note: on OSX there is a bug where your part will appear floating above the page. You can close the part using the button at the bottom of the screen and it should disappear.

Select the final operation that completed the part, and then press this button to add orthographic drawings of our part to the page.

Choose these options. Our part was drawn with –Y to be the front, so choose View from: -Y. (If this isn’t the front of your part, pick the correct axis). Add three secondary views, including one isometric view (checkboxes). Press ok.

In my software, the views are too large and overlap. This is fixed by expanding the “Page” in the model browser, selecting each view, and then changing the scale from 2 to 1.

Now that we have the views, we need to add dimensions and then write our name on it. Before dimensioning, it should look like this. The views are, clockwise from top left, Top View, Isometric View, Side View, Front View.

Now use the following tools to add dimensions. Note that you cannot add correct dimensions on the isometric view, only on the front, top, and side.

Click a side and place a label with the length.

Click two sides, two points, or a point and a side. It will create a label with the distance between them. Note: there is a bug on OSX where after creating a dimension, you cannot delete it unless you delete the entire page.

After labeling sufficiently so that every dimension on the drawing can be at least calculated from the other dimensions, my result is the following:

Note that there are no measures on the angled faces, because the tool cannot do it.

To save this drawing, press the Export to SVG button. SVG is a vector graphics format, it is an

image that is defined by points and lines.

Now the last step is to put our name on it. We couldn’t change the text in FreeCAD, but we can edit the

file in Inkscape. Open the SVG in Inkscape.

Use this text tool to click on the text fields and change them to your name, add a drawing title,

etc. Inkscape is a powerful tool and you can make other edits as you wish, such as changing text, line

styles, moving your drawings around to make the result more attractive. For instance, I quickly corrected

the placement of one label that was partially obscured.

The final product:

This can be exported as an image for printing by using the Export PNG tool. Make sure you choose to export the entire Page. Set the DPI to 150 for printing, or 96 is enough for sharing online. Choose the path under Export As… Finally, don’t forget to press Export, or else it won’t save.