Catia v5 Tutorial: Lumber Axe - Part 1

By the end of this Catia tutorial, you will be able to:

- Assemble different parts into one assembly.
- Get a better understanding on fillet and chamfer function.

In this tutorial, we will be creating an axe based on this picture which I have found on the net:


Instead of creating the whole axe in one go, we'll be creating two separate parts:

1. The axe head - which is the metal part
2. The axe handle - which is the wooden part.

After creating this two parts as a separate project, we will assemble them using the Assemble Design option. For now, just forget this and we will get back to it once we have created the two parts.

Okay, let us get started. Start by starting up Catia and opening a new Part Design file (Start > Mechanical Design > Part Design) and name the part "Axe Head".

Select the yz axis and select the Sketch tool. Draw a sketch of the axe head according to the picture below:


Use the Spline tool to draw the curve line on the left side of the sketch. Place the three points as where they are in the picture. You can use the Line tool to draw the rest of the straight lines.

Once you have finished drawing the sketch, select the two straight lines at the bottom of the sketch. We are going to smoothen the edge by giving it a nice corner. While still selecting the two lines, select the Corner tool, type in 100mm as the radius and hit the "Enter" button on your keyboard. This will make the sketch look more like a axe head instead of that sharp edge.


As you may have noticed in the picture of the axe above, there is a curve part near the place where the axe handle connects with the axe head. That is what we will be doing next.

Select the Circle tool and set the circle center at 160mm for the horizontal axis and 60mm for the vertical axis. That would put the circle center somewhere in the middle of the bottom line. Next, set the radius of the circle to 30mm.

Now, we will want to delete the top half of the circle and part of the straight line which is in the circle. To do this, we will need to use the Quick Trim tool which can be found under the Trim tool. You can find the Trim tool in the Operation toolbar.


Select the Quick Trim tool and select the lines that we want to delete which was mentioned earlier. After deleting the lines, your sketch should look like in this picture:


Exit the workbench and select the Pad tool. Set the Length to 10mm and click OK. Select the curve edge and select the Chamfer tool. In the Chamfer Definition window, change the Mode to Length1/Length2. Set Length 1 to 10mm and Length 2 to 100mm. Leave the rest as it is and click ok. We have now created the bit for the axe head.


Next, we are going to smoothen the face of the axe head. Select the line as is shown in the picture above. Select the Fillet tool and set the radius to 600mm and select OK.
Select the top surface of the axe head and select the Sketch tool. We are now going to create the hole in the axe head where the axe handle sits. Instead of using the Rectangle tool, we will use the Centered Rectangle tool. Click the arrow next to the Rectangle tool to bring up a list of other tools. The second last tool on the right should be the Centered Rectangle tool. Select it and set the First point at H: 0mm and V: 160mm. The center of the rectangle should be at a fix position. Next, set the height to 64mm and the width to 12mm and hit the "Enter" button.


Exit the workbench and select the Pocket tool. Set the Depth to 90mm and select OK. Select the two corner in the pocketed area and select the Fillet tool. Set the radius to 1mm.


Once you have done that, fillet the top part of the circle and set the radius to 3mm. After that, fillet the two ends of the circles with radius set at 2mm.


It should be looking like this after you have finish filleting:


As you may have noticed, up till now, we have just created half of the axe head. Instead of creating the whole piece from scratch, we just have to create half of it and later mirror the half to create a complete head. That is what we will be doing now.

At the tree, select the Part Body. This action will highlight the whole axe head that we have just created. Now, select the Mirror tool and select the yz plane. This will mirror the object with respect to the yz plane. If you can't find the Mirror tool, it can be found under the Transformation Features toolbar. After that, select the butt of the axe and select the Fillet tool. Set the radius to 2mm to make the butt less boxy.


If you have done everything correctly according to this tutorial, your axe head should be like in this picture:


That is all for now. I'll post the tutorial for the axe handle another time. Till then, see ya.

Make sure to check back for future updates in Catia v5 Tutorial for Beginners.

Catia v5 Tutorial: Fillets and Chamfer

We'll be using the box that you have created according to the previous tutorial.

I hoped that you did remember to save the previous project onto your hard drive. Else, you can visit Getting Familiar with Catia v5 to create the box from scratch.

We will now start with chamfering the base of the box. Select the surface under the box and click the Chamfer tool.


If the bottom surface is hidden from your view, you can select the Rotate tool. You can drag the screen around using the Pan tool. If you need to zoom in or out, you can use the Zoom tool. All of these tools are located at the bottom toolbar.


Another alternative to these three tools is by clicking the scroll button on your mouse and moving it around. I have listed the combination for each of the functions below:

scroll button = Pan
ctrl + scroll button = Zoom
scroll button + ctrl = Rotate

These shortcuts are live savers. Trust me when I say that. In future projects, you'll be needing to pan, rotate and zoom a lot. With these shortcuts, you wouldn't need to reselect the Pan, Rotate and Zoom tools again and again. You can also use the Axis to have a more controlled rotation as it rotates only on one axis at a time.

Okay, now back to the project. After selecting the bottom surface and Chamfer tool, a Chamfer Definition window will appear. Set Length 1 to 40 mm and leave the rest as it is. Select Preview to view the outcome and click OK.

You will notice that the base of the pocketed area is showing. No worries. This can be solved by chamfering that area too. To chamfer this area, just repeat the previous steps. This time, set Length 1 to 30 mm instead.

Your chamfered box should be looking like this now:

Notice how all the edges are pointy sharp? With little effort, you can make this box look much better. Now, we'll begin filleting the edges.

Since we will be filleting all the edges, you can start be selecting any surface. Then, select the Fillet tool. In the Edge Fillet Definition window, set the Radius to 3 mm. Select OK and do the same for all other surfaces.

There are a few ways to fillet an object. You can either

1. Fillet a line by line
- use this when each line has different fillet radius.

2. Fillet surface by surface
- use this when lines on the a surface have different fillet radius from other surfaces.

3. Fillet the whole object at once
- use this when all the lines on every surface have the same fillet radius (like the project that we are doing now).

Once you are done filleting, your box should be looking like this:

I know. It looks even horrible with all those lines then before the filleting was done, isn't it? No worries. The next step that we'll be doing will solve this problem for us.

At the bottom toolbar, look for the Shading with Edges tool. Select the tool and it will expand, offering us with several tool for us to choose. Select the Shading with Materials tool. Your final product should be like this:

Notice how your box look much neater then before? You can play around with the Shading tool to see the appearance of each of the tools.

With that, thus ends the tutorial for chamfering and filleting.

Make sure to check back for future updates in Catia v5 Tutorial for Beginners.

Getting Familiar with Catia v5

So where do we get started with Catia v5?

Well, the very first thing to do, obviously, is to get the software started.

At the top left corner, select Start > Mechanical Design > Part Design.

(Click to enlarge)

A New Part window will appear. Replace Part 1 with whatever you want to name your file. For now, let's name it Box and select the OK button.

On the left side of the screen, you will see the tree which will list
all the parts of your drawing. Select the xy plane and then
select the Sketch tool. This will bring up a screen filled with grids and this is called the Workbench.

Select the Rectangle tool which is located on the Profile toolbar on the right side of the screen. If you can't find it there, just click and hold the left button while dragging the toolbar onto the screen until the Profile toolbar appears.

Once you found the Profile toolbar, select the Rectangle tool and draw a rectangle with a length of 300 mm and height of 200 mm (One small box is equivalent to 10 mm). Then, select the Exit Workbench tool to return to the 3D view.

While selecting Sketch 1 on the tree, select the Pad tool. A Pad Definition window will appear and set the length to 100 mm. Click Preview to see the result. If you are satisfied with the result, click OK. Now you have created an oblong.

Select the top surface of the oblong and select the Sketch tool. Now select the Rectangle tool and draw another smaller rectangle within the surface.

Exit the workbench. While selecting the rectangle which you have just drawn, select the Pocket tool. A Pocket Definition window will appear. Set the depth to 90 mm and select OK. If you have followed the steps earlier, your box should be looking like in the picture below.


You have now created your first object using Catia v5.

Remember to save it just like how you save other files.

That's all for now. See you in my next tutorial. Till then, familiarize yourself with Catia v5 by playing around with it.