How to Complete Your CAD Homework

Models like this are common homework assignments for CAD students. Let's learn some skills to convert an isometric drawing into a 3D model.
SOLIDWORKS is used, but these skills apply to any 3D CAD program.

  1. Step 1: The Assignment

    Convert the above image into a 3D CAD model

    This model and image can be found in the GrabCAD Library. You won't need it though, because this tutorial will show you strategies to model hundreds of similar models on your own.

  2. Step 2: It's Simple, but Complex

    Ask anyone who makes CAD models for a living if this model is difficult, and they will laugh. This model can be made in minutes (once you have a year or two of modeling experience).

    If you are just starting out, don't be discouraged. There is a lot of "stuff" going on in such a simple model. Many experienced users and instructors (mistakenly) assume you already know this information.

    Let's consider some knowledge you need to solve this assignment:

    ·       What is the front view?

    ·       What does this part look like from other views?

    ·       What are the units of measure?

    ·       What (if any) assumptions need to be made?

  3. Step 3: What is the Front View?

    Generally, the front view provides the most information.

    When an isometric view is show, the front, top, and right views are laid out as shown above.

    A modern drawing will usually shown the three standard drawing views, and the isometric view. A "simple" part like this could be represented with a single view, but it is an uncommon drawing method now. This type of single view, isometric drawing was common decades ago when each view was drawn by hand.

    In the above image a typical modern drawing is shown. This drawing is created using the Third Angle Projection method (common in the United States). Before creating a drawing, determine if you need to use Third Angle, or First Angle Projection (common in the rest of the world). Wikipedia has a great entry on the topic.

  4. Step 4: Unit of Measure?

    In the United States, inches are the standard. The rest of the world has unified on millimeters.

    A drawing should state the units of measure, but remember that we're not dealing with a "real drawing" for assignments like this.

    One method to determine the units is to imagine what this part might be used for, then look at the overall dimensions used. In the image above the overall dimensions are 110 wide by 45 deep by 62 high. Is this a part you can hold in your hand? Or is this a part which you can climb on? 1 inch = 25.4 mm. I'm 72" tall (1,829 mm). Can I hold this part? Or is it bigger than me?

    Another hint to determine the units used can be found in how the dimensions are written.

    For drawings in inches the following are true:

    ·       Dimensions smaller than 1" do not show a leading 0. There are no units above smaller than 1, but if there were (and inches were used) they would be displayed as .25 NOT as 0.25

    ·       Units larger than 1" will show a number of trailing zeros to indicate their general tolerance. This means a unit like 110 would be displayed as 110.0 or 110.00 or 110.000 depending on how tightly toleranced the dimension needs to be.

    For drawings in metric units the following are true:

    ·       Units under 1 have a leading zero as a prefix. Therefore .25 would be displayed as 0.25 on a metric drawing.

    ·       Units of a whole value larger than 1 do not display trailing zeros. Therefore 110 would be displayed as 110. NOT 110.0

    Based on the above guidelines it should be clear that metric units are used in the assignment.

    If you use the wrong units to create your model, there are some options:

    1. Remake the model using the correct units. A model like this should not take more than an hour to produce. It will be even faster the 2nd time. And you need the practice.
    2. Insert a Scale feature at the end of your model to scale the model as needed. This is a terrible solution, but it is slightly better than having a model that is 25.4 times too big.
    3. Create (or find online) a macro which will scale every dimension in every sketch and feature as needed to produce a model of the correct size.

  5. Step 5: Assumptions Needed?

    There are some assumptions needed to complete this model. Can you identify them?

    1. Does the 60 mm wide opening on the bottom go all the way to the back of the part?
    2. Do The four Ø12 mm holes go through the part?

    Ideally the callout (Ø12 X4 HOLES) would have a note to indicate they are THRU holes. But, since no information is provided to indicate a depth other than all the way through, we'll take an educated guess and make all holes and pockets go through the part.

  6. Step 6: What About the Origin?

    We've determined the correct unit of measure, and know what the standard drawings views are supposed to look like. The last piece of information needed before a model can be made is:

    Where does the origin go?

    The origin is the fixed point in the CAD system located at the intersection of the three primary reference plane (front, top, right). The origin has a coordinate position of 0,0,0 in the model space.

    Where should the origin go?

    This is a hard question to answer for two reasons.

    1. It varies with every model.
    2. It really doesn't matter (most of the time).

    To resolve the first issue above, we'll focus only on this model.

    To resolve the 2nd issue, there are a number of bad places to put the origin, and a number of better places to put it. But, even if you pick the wrong location, it is possible to add another origin to the model later. And sometimes you may want multiple origins (an example is using one for CAD modeling, but a different origin to indicate the part in CNC equipment).

    In the image above I've indicated several locations that make sense for the origin. Which is "the best"? It really depends on a lot of factors which won't be covered until later in your schooling.

    As a general rule, I put the origin in the middle of a symmetrical part. For my model, I used the location indicated by the dot in the center of the part directly over the 60 mm dimension.

  7. Step 7: The CAD Model Recipe

    Have you ever followed a cooking recipe? Many times there is a sequence to follow, but there are some steps which must be followed in the correct order.

    CAD models work the same way. There are guidelines which should be followed for most models.

    ·       Add material, cut away material, add little details (i.e. fillets and chamfers).

    ·       Keep sketches simple. Don't try to make multiple features with a single feature.

    ·       Try not to start your model by sketching a rectangle.

    ·        There isn’t a “right way” to make a model, but there are better (and worse) ways.

    ·       Symmetrical parts should be centered on the origin.

    Above are the seven steps I used to create this model. Notice I started with an "L" shape instead of a rectangle. I broke the rule about putting fillets last. But the drawing locates the four holes concentrically with the filleted corners, so that's how I made the model.

    Is this the "Best" way to make the model? It does not matter. If the model is correct, easy to edit, and built in a logical sequence, an argument for it being wrong, or bad can't be made.

    "What about feature count?" Some people are obsessed with feature count, I'm not. Especially for simple models like this. Reducing feature count usually leads to more complex sketches which perform multiple operations at once. This means the model is more difficult to edit later.

    Reducing the feature count from 7 to 5 (image above) creates a more complex multi-profile sketch for the third step. If you are later asked to suppress (turn off) one or more of those individual cuts, the process would be more difficult when compared to the seven step example above where each cut is made with a separate feature.

    Below is an image of the feature tree from the 7 feature model. For some models you may want to experiment with renaming these model features. Boss-Extrude2 can be vague. Naming it "V Shape" may make identification easier if you or someone else needs to edit the model later.

    It will take some time to develop an eye for it, but creating a CAD model is all about breaking the part down into smaller, easy to make features.

  8. Step 8: Checking Your Work

    Making a model is a waste of time if the end result is incorrect. One way to prevent errors is checking your work as you create the model. Here's how I do it:

    Have a copy of the drawing open while you work. This can be on another monitor, a printed sheet of paper, or in another program in the background. As I create a model from an image, I cross each dimension off the drawing to indicate it has been used. Here's an example:

    You never know when you might need a previously crossed out dimension to help determine an unknown value with some simple math, so try to keep the values legible.

  9. Step 9: Single Monitor?

    Most of the work I do at home is done on a laptop with a single monitor. This leads to constantly using Alt + Tab to cycle between SOLIDWORKS and the drawing. One trick to see the drawing in SOLIDWORKS while creating it is to insert the drawing into the part you are making.

    The above does not help with crossing off dimensions as they are used, but it reduces the chance of forgetting the value, or using it in the wrong location.

    Here's what it looks like:

    Even better is that as the CAD model is rotated, the image remains static so it can always be read:

    Here's how to get a picture into your CAD model as shown above:

    1. DON'T use Tools - Sketch Tools - Sketch Picture. This is a great tool, but it place the image on a plane. The image will rotate with the model and be impossible to read at times.
    2. You can try to use Insert - Object. This often does not work correctly, and you'll be left with an icon representing the image instead of an image.
    3. To get it to work reliably, Open the image in a viewer or editing program, copy the image (i.e. Ctrl + C), then inside of SOLIDWORKS, paste the image (i.e. Ctrl +V).

    Below is an example of what happens when SOLIDWORKS decides to place an icon into the part instead of the picture:

  10. Step 10: Bonus Points (and Fun)

    Making CAD models should be fun. If not, you might be studying for the wrong profession.

    When your 3D model is complete, and you've checked it for errors, make a rendering of it. Rendering an image makes it look much better by applying realistic materials, backgrounds, and lighting to and around the model.

  11. Step 11: Cheating?

    Can you cheat in a CAD class? Maybe. But, it can be difficult.

    Chances are you are using an educational version of the software. This usually means you won't be able to open/import a model created in a commercial seat of the software. You could import a generic model like a Step, Parasolid, or Iges file, but those will import without a feature tree.

    3D models are also tagged in their properties with the name of the person who created them. An easy to overwrite tag is located in File - Properties - Summary. This simply shows the login name of the last person to save the file.

    Another user name and time stamp is added to every feature in the feature tree. Right click a feature and choose Feature Properties. The name and time of creation is saved there. If your instructor is smart (or they read this tutorial), they'll be able to easily spot a model made with another person's name.

    Also consider that it is unlikely that two students would make this model in exactly the same way. There are so many variables from reference sketches, constraints, and face names, that two people having the same model is VERY unlikely. Models are like handwriting, or voices. They can be similar, but can be individually identified by unique characteristics.