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Rapid Design through Virtual and Physical Prototyping

IronCAD Lab - One

This lab is derived from the IronCAD tutorials. The help files and Show_Me files are on the cluster computers. These help files are actually helpful (unlike MicroSoft help). So if you want to find out how to use the Sheetmetal functions in IronCAD, search for Help on sheetmetal.

1. Getting started

Select IronCAD from the Start -> Programs -> CAD menu. The IronCAD logo is a black I-beam on a red background:

Once you start IronCAD, you will get the following window:

Select Create a new Scene and click OK. (Drawings are 2D and Scenes are 3D.) You will get another dialog box. This box lets you select the background color and whether or not a grid (drawing plane) is displayed. Select an option with a grid.

1.1. Drag and drop editing

Before we start, move your mouse to the menus at the top of the screen. Look at the options in each of the menus. We will use only a few of these commands in the introduction, but looking at the menus will give you a sense of the options in IronCAD.

After you make a selection, the menu on the right will disappear. Move the mouse close to the tab that says Shapes. The shape menu (which you can see on the above) will reappear.

In the Shapes menu, click on the Block shape. Without releasing the mouse, drag the block into the scene. As you drag the mouse over the scene, a small block will follow it. (I can't show you this in a screen dump because the cursor doesn't show up in screen dumps.)

Release the mouse. You will have a block in your drawing. Click twice on the block. Notice that the edges of the block are yellow. Yellow means that the part is selected.

Move the mouse around the handles (red balls) on the block. You will see the cursor change shape and the handles change color. Put the cursor over the top pin until it turns yellow when the cursor turns into a hand with a two headed arrow under it:

move the cursor up and down. The part will resize along the selected axis.

Do the same with one of the handles for the x or y dimension.

1.2. Moving around

To get a better view of your block, go to the menu on the left and click on the fit scene button:

While you're looking for this button, hold your cursor over the other buttons to see the other ways you can change your view of the scene. Try the dolly camera, orbit, pan and zoom buttons. You probably have a strange perspective on your block now. You can press the restore camera button, which will return the view to the standard perspective.

To get a view of the whole block, press the fit scene button again.

1.3. Undo and redo

Since you have performed several operations on the block, go up to the tool buttons and press the Undo button until your block disappears.

Press the redo button until it is back to its final shape. Notice that undo and redo only operations on the geometry. They don't undo/redo changes in the view.

1.4. Adding shapes

Go back to the shape menu on the right hand side of the screen. Select the cylinder shape and drag it into the scene.

Don't release the cursor yet. Move the cursor around the faces of the block. As you move near a face, the edges of the face turn green and the center of the face is highlighted:

With one of the faces highlighted, release the mouse. The cylinder will be added to that side. The handles of the cylinder are automatically selected so you can reshape the cylinder.

After you are done reshaping the cylinder, click in the background. You can also add another cylinder to the scene that is not connected to the block. Drag another cylinder in, and drop it away from the block. Be sure that no points or faces on the block are highlighted in green.

IronCAD also has negative (H) shapes. Select an H-slot from the Shapes menu and drag it and drop it onto another face of the block.

Add some more positive and negative shapes to your part: Orbit your part and add/subtract shapes on all the sides. To see what you have added to your part, and to make it easier to select a particular sub-shape, click on the scene browser button.

You will get a window on the left-hand side of the screen that shows you the composition of your parts. Click on one of the shapes, and it will be selected in the scene.

2. Making 3D shapes from 2D cross sections

Making parts using the standard shapes (called primitives) is easy, but you won't be able to make all the shapes you want that way. Sometimes, you will need to draw a profile and then extrude or rotate it to make a solid part. We will only make solid parts in this class, because our goal is to make parts that can be manufactured on the rapid prototyping equipment. IronCAD, and most other CAD programs, also enable you to make 3D surfaces, but we will not cover them in this class.

2.1 Creating a 2D cross section

Since IronCAD only lets you create valid 3D parts, you can't just draw in 2D. To make a cross section, you need to start by stating your intentions. We are going to make a balloon. My plan for the balloon is to make a profile that looks something like the following:

and then revolve it around the vertical axis to make a solid balloon. This is called a Spin Shape in IronCAD. In the toolbar, you will find a set of buttons that let you extrude, spin, sweep and loft. Press the Spin Shape tool button.

You will get a sequence of pop up windows with the options for creating cross sections. For all but the third menu, the defaults are fine.

For the 3rd step, I changed the major grid line spacing to 0.50 inches and the minor grid line spacing to 0.01. inches.

You will get a grid in your drawing space and pop up toolbar for creating the profile:

Before we draw the profile for the balloon, let's look at some of the formatting options for the grid. Select Format -> Grid.

Note that this menu item is only available when you are creating or editing a cross section. When you select this item, you will get a popup window that lets you control how the cross section is created. The screen dumps below show the options for each tab in the Drawing Options window.

When you are done selecting the options you want, click OK. You will now have the grid in your drawing area. Use the magnify tool on the left to zoom in on the grid. I prefer the magnifying tool that let's me select the window to zoom in on, but you should experiment with the different zooming options to see which one works best for you. Once you have zoomed in on the grid, select the polyarc tool from the bottom toolbar. This tool will let us create a sequence of arcs.

First, I clicked on the W axis to start the balloon. Then, I moved the mouse around until I got an arc that looked right for the balloon:

I clicked to make the arc, but because this is a polyarc, I can keep clicking to make new segments of the the polyline:

Next, we want to make a series of lines that close the bottom of the balloon and form the stick that the balloon is on. Press enter to end the polyarc and press the polyline tool to start a sequence of lines. In the options for the grid, we selected snap to geometry, so if you put the mouse close to the end of the last arc and click, the end point of the arc and the start point of the line will be the same point. This is important because otherwise the balloon would have a hole in it and we wouldn't be able to revolve it. I clicked the mouse to make a sequence of lines including one along the axis (which doesn't show in the screen dump) to create a closed cross section of the balloon.

When you are creating a cross section, you may get an error message like the following:

To repair the problem, select Edit cross-section. You will get a view that lets you move the points around until the profile is valid.

When you have a valid cross section, select Finish Shape from the cross section window. The cross section will revolve around the axis and you will have a solid balloon:

However, if you zoom out, you will see that the balloon is lying along the y axis. To rotate it to the z axis, we are going to use the triball. The triball is a 3d manipulation tool that is very powerful, but takes a while to get used to. Select the balloon and then click on the triball tool button:

The triball will appear on the part:

I have included the IronCAD help pages on the triball and some slide shows that take you through the steps of different operations using the triball, so I will not include that in this part of the tutorial.

Select the x axis in the inner part of the triball. It will turn yellow. This means that the axis is frozen - so we will be able to rotate the part around the x axis and swing it up to the z axis.

Move the mouse on the inside of the triball until you get the rotation hand:

Move the mouse and the part will rotate. We want to rotate exactly 90 degrees, but it's hard to stop at exactly 90°.

Right click on the numerical value of the angle. You will get a menu that lets you edit the number:

You can enter 90 in the window that opens.

Note: We could have avoided this final rotation step by selecting the z axis before we started the spin shape. To select the z axis, (or whatever axis you want to rotate around) just click on it.

Next, let's move the balloon up in the air. The outer handles on the triball are used for translation. First, lock the z axis by clicking on the outer z handle. It should turn yellow.

Grab the top handle with the translation hand.

Pull up on the handle until until the balloon is about 1 unit about the x-y plane

Right click on the numerical value and select edit distance. Make the distance 1.

Finally, right click on the balloon and select SmartPaint from the menu.

In the Smart Paint window, you can select a color for the balloon, you can make it shiny, you can make it slightly transparent, you can put a decoration (decal) on it, and you can make it glow slightly. Play with the options to see how they change what the balloon looks like.

3.Dimensions

In the first section, we just dragged in parts and resized them without any sense of their true dimensions. This is not the way one normally designs a part. Let's start a new scene. Our goal is to make the following part:

This part is made up of two plates joined by a cylinder with holes in the corners of both plates. The corners of the plates are rounded. We will start by making the bottom plate with the dimensions 4.724 x 4.724 x 0.197. Then we will make a cylinder with an inner radius of 2.212, an outer radius of 2.527 and a height of 0.591.

First, select File -> New and select Scene from the dialog box.

You will get the menu that lets you select the background color and a grid. This time, select an option with a grid. You will see the x-y plane with a basis vector at the origin.

3.1. Units

In order to dimension something, we need to know what the units are. Select Format -> Units. You will get the following dialog box. The default units for IronCAD are English units: Inches, Degrees and Pounds. Look at the pull down menus to see what the options are for each attribute.

Since the part we are drawing is in inches and degrees, click OK.

3.2. Viewing and editing dimensions

Drag a block into the scene again. Now select View -> Sizebox dimensions. Click to select the block so it turns yellow, and you will see the dimensions.

Now grab one of the handles. As you resize the block, you will see the dimensions change. This doesn't seem like a very accurate way to dimension a part. Select one of the handles, and right click on the handle. If you select a face or edge instead of a handle, you will get a different menu. Be sure that you have a handle selected before you right click.

You will get a box that allows you to change the length, width and height of the box. How do you know which way the dimension will change? It will change the dimension in the direction of the handle that you selected.

Change the length to 2.5 and press OK. IronCAD changes the length of the box to 2.5 by moving the left-hand face. Select the same handle again, but this time change the other dimensions:

This time, IronCAD resizes the block around the anchor (the pin in the blue/green dot).

3.3. Specifying the resizing behavior

The default for IronCAD is to scale from the opposite face, but you can change this behavior. Right click on a face of the block and select Intellishape Properties.

You will get a dialog box with many tabs. Take a minute to look at the options in the tabs. When you are done, select the Anchor tab. This tab tells you the location of the anchor. The height should be zero (i.e. the anchor should be in the x-y plane. The anchor should be located at the mid-point of the length and the midpoint of the width.

Now select the Sizebox tab. Notice that you can change the length, width and height of the part in this menu. We are going to change the default behavior of the resizing operation. Pull down the menu next to Length and select About anchor.

Click OK. Grab the left-hand handle again. As you move the handle, you will see that IronCAD now resizes the length around the anchor rather than from the opposite face. Since we didn't change the resizing behavior for the width or height, they will still scale from the opposite side. After you understand how this works, go back to the Sizebox menu. (Right click on a face and select IntelliShape Properties.) Make the default behavior to resize from the opposite handle.

Select the handle on the top face of the block and right click. Since we have selected this handle, IronCAD will resize the block relative to the opposite face. Since the opposite face is sitting on the x-y plane this is what we want. (If it resized it about the anchor, the part would extend in the negative z direction.) Set the height of the block to 0.197.

Click OK.

Now we need to change the dimensions of the length and the width. We want to scale these around the origin, which is the default for the non-selected handles in the sizebox. So, select the top handle again and right click to get the edit window for the size box. Change the width and length to 4.724.

Press the fit scene button if your part goes off the screen.

We will add the cylinder and top plate before we chamfer the corners and add the holes.

4. Modifying shapes

4.1. Combining shapes

Go to the Shapes menu and select a cylinder. Drag it to the plate. As you drag it close to the center, the green dot will become brighter. Drop the cylinder when the dot is highlighted. Press the fit scene button.

Notice that because earlier we selected the option to show the dimension box, the dimensions are shown for all selected parts now. You can toggle this option on and off depending on what you are working on.

Select the top handle and right click to get the edit sizebox window. From the drawing, we know that the height of the cylinder is 0.591 and the outer radius is 2.527. In the sizebox, set the height to 0.591. (Which direction will it scale in?) Since the radius is 2.527, the width of the cylinder is twice that. IronCAD will do the arithmetic for you, so you can enter 2.527*2. As soon as you enter this, the length will change to the same value since the length and the width of a cylinder have to be the same.

We still have some work to do cleaning up the cylinder and making it hollow, but before we do that, we are going to add the plate on the top. Select another block from the Shapes menu. Drag it to the top face of the cylinder and drop it when the green center dot is highlighted.

4.2. Smart snap

We could size the new block the same way we did the first one; however, IronCAD has an extremely useful feature, called Smart Snap, that we will illustrate with this part.

Hold the shift key down and pull on the left-hand handle. As you pull it toward the edge, you will first see the edge of the cylinder highlighted and then the edge of the bottom plate.

Release the mouse when the edge or face of the bottom plate is highlighted. The face of the new block is now co-planar with the face of the lower block. Do the same thing with each face. Use the orbit tool to see and change the other faces.

Now all we have to do is change the height of the top plate. Select the top handle. (Which direction will IronCAD resize in?) Right click and change the height to 0.197.

4.3. Subtracting shapes

Next, we want to get rid of the material of the cylinder that's hanging out over the edges. What we are going to do is to use a negative block (H-block) and put it where we want to remove the material. Go the Shapes menu and select an H block. Drag it to the left hand end of your part. Drop it when the green dot at the midpoint of the edge is highlighted. (The screen dump of this doesn't show anything interesting. You will just have to do it.) When you drop the H-block, IronCAD will take a chunk out of the part. This is not what we want!

Select the H-block. (If you can't select it, select the scene browser and select the H-block from the tree.) Drag the left hand face of the H-block to the left. Drag the bottom face so that it extends beyond the bottom of the part. Now we are going to use Smart Snap again. Press the shift key, and drag the right-hand handle toward the edge of the part. When the edge of the lower plate is highlighted, release the mouse. The negative block has subtracted the overhang. Perform the same operation for all the sides. (If you watch the tutorial, you will learn how to use the IronCAD triball, but this lab is getting long, so you can do that on your own.

Now let's make the hole for the center of the cylinder. Go to the Shapes catalog to the right of the drawing area and select the H-cylinder. Drag it and drop it on the center of the top plate. Be sure the green dot that marks the center of the top face is highlighted when you drop the shape.

The inner radius of the cylinder is 2.212. So, select the top handle and right click to get the size box. Enter 2.212*2 for the width of the H-cylinder.

After you press enter, your part should look like:

5. Views, textures, colors, ...

To get standard views of your part (e.g. top, right, isometric, etc.), select Tools -> Standard Views. You will get a separate toolbar that has buttons for the standard views.

Using this toolbar should make it easier to get the view of your part that you want.

Here is my final part after I applied the blend, dragged the fire texture to the surface of the part, and selected the standard isometric view.

To see other options for the color of a part, right click on the part and select SmartPaint from the popup menu.

As you go through the SmartPaint tabs, you will see that the fire texture is implemented as a reflection on a solid white surface. Try changing the color, finish, transparency, emission, etc. of your part. You can click the Apply button to see the effect of the change without closing the menu.

Note: If you have only one face selected (i.e. the face outline is highlighted in green), the color changes will apply only to that face. In the following screen dump, I made one face flat green, another face 50% transparent blue and applied the play decal to the third face:

Note: You should not paint your parts like this!

sfinger@ri.cmu.edu