Catia v5 Tutorial for Beginners

Catia v5 Tutorial: Measurement Units and Grid Spacing

2012-07-03T13:44:00.002-04:00

The default measurement unit that comes with Catia v5 is in milimeters (mm) and the spacing for the grids are 1 mm for major grid lines (or also known as Primary Spacing) and 0.1 mm for minor grid lines (or Graduation).

However, as you may have noticed, the Catia v5 Tutorials that is available here uses inches (in) as their measurement unit. In order to adjust the measurement unit to the one that you desire, all you have to do is to access the Options window located under the Tools menu.

In the Options window, select Parameters and Measure which in located on the Options tree. In there, select the Units tab and you will be presented with all the parameters available in Catia v5. Select the parameter that you want to adjust and for this tutorial purpose, we will be changing the units for Length. Once you have selected a parameter, you can change its units by using the drop down menu.

In the Sketcher menu, under the Mechanical Design tree, you can adjust the Primary Spacing and the Graduation values to suit your preference. As mentioned earlier, Primary Spacing is basically the length of each major grid lines while Graduation is the spacing between minor grid lines.

As you can see below, I have set my Primary Spacing to 1-inch and the Graduation to 10. This basically means that the length of my major grid lines will be 1-inch while the minor grid lines are 0.1-inch.

I hope that you found something useful in this tutorial. Make sure to check back for future updates in Catia v5 Tutorial for Beginners.

Catia v5 Tutorial: Pattern and Mirror

2012-07-03T01:30:00.001-04:00

In this tutorial, we will incorporating several tools, which had been gone over in previous tutorials, into one part.

In addition to that, we will also be covering two new tools in this tutorial. The Pattern and the Mirror tool.

As in previous tutorials, we will still be working in Part Design. We will start by creating a 5-inch by 5-inch square in Sketch on the xy-plane. For this square, make sure that one of its corners coincide with the origin of the axis.

Exit the workbench and create a Pad of 1.5-inch. Next, we will create the feature in the following image on the box that we have just created.

There are two simple ways to create this. One way is using the Pocket tool and the other is to use the Shell tool.

To use the Pocket tool, you will need to create a sketch on the top surface of the box. Just select the Sketch tool and select the top surface as the plane for your sketch. Create a square within the boundary of the original square with 0.2-inch gap from each sides.

Exit the workbench. While selecting the sketch that was just created, select the Pocket tool. In the Pocket Definition window, set the Type to Up to Last and set the Offset to -0.2-inch.

The other way to do this is to use the Shell tool. For simple and constant wall thickness such as the one that we have for this part in this tutorial, the Shell tool is slightly faster and convenient than the Pocket tool. To do so, select the Shell tool and choose the top surface as the Faces to Remove and set the Default Inside Thickness to 0.2-inch.

Which method being used does not really matter in this particular tutorial since both methods produce the same shape results that we are aiming for.

Next, we will create fillets on the inside of the box. Select the edges highlighted in red. To select multiple elements at the same time, hold down the Ctrl button on the keyboard and select the desired elements. Once you have selected all the highlighted edges, select the Edge Fillet tool and set the Radius to 0.2-inch.

Next, we will be using the Mirror tool to create a pattern using the box that we have just created. Select the Mirror tool and select the left side of the outer surface.

Select the Mirror tool again, and this time select the back side of the outer surface.

What you will end up with now, is a larger box with four identical compartments.

Another method of creating this four-compartment box is using the Circular Pattern tool. This can be found in the extension under the Rectangular Pattern tool. In the Circular Pattern Definition window, set the Parameters to Complete Crown and Instance(s) to 4. Select the edge highlighted in orange as the Reference Element.

We will now create a circular hole of 0.5-inch in the center of one of the compartments. Select the surface highlighted in orange and select the Hole tool. In the Hole Definition window, set the type to Up to Last. Before pressing the OK button, click the Positioning Sketch button to align the hole to the center of the compartment.

After selecting the Positioning Sketch tool, you will be brought into the workbench with a center point which indicates the position of the circle. To align the point to the center of the compartment, just create a constraint between the point and the sides of the compartment.

As you may have noticed, the constraints are purple in color. This indicates that the profile is over constraint. If you try to change one of the constraint value, you will encounter an error. In order to avoid this, just pick either one of the constraint and set it as a reference.

You will notice that the constraint chosen as a reference will have a parenthesis around its value. The value of this reference constraint will change according to the changes in the other constraint. To set the center point of the circle in the center of the compartment, you can use a simple average equation in the Value blank in the Constraint Definition window.

Repeat the same steps for aligning the center point with the other sides.

Next, create another 0.5-inch hole on the same surface with the following constraints.

After that, select the Circular Pattern tool and select the second hole that was just created. In the Circular Pattern Definition window, set the Parameters to Complete Crown, Instance(s) to 6, and the first hole as the Reference Element.

Finally, we will repeat the hole patterns that was just created to the compartment which is diagonal to the original compartment.

To do this, we will make use, once again, of the Circular Pattern tool. In the Circular Pattern Definition window, set the Parameters to Instance(s) & Angular Spacing, Instance(s) to 2, and Angular Spacing to 180 deg. Select the circular pattern that was created earlier as the Object and select the top surface the box as the Reference Element.

To complete the part, repeat the same steps for the center hole.

In this Catia v5 tutorial, we have used Pad, Pocket, Shell, Edge Fillet, Hole, Mirror and Circular Pattern all in one part.

As mentioned earlier with the Pocket-Shell and the Mirror-Circular Pattern method, either methods produce the same outcome for this particular tutorial. In order to create a certain shape, there will be numerous methods to obtain the same final outcome. Therefore, it is mostly always best to use the most convenient and simple method to minimize complexity.

I hope that you found something useful in this tutorial. Make sure to check back for future updates in Catia v5 Tutorial for Beginners.

Catia v5 Tutorial: Multi-section Solid and Shell

2012-06-27T09:45:00.000-04:00

In this Catia v5 tutorial, we will be going over the Multi-Section Solid and the Shell tool. The Multi-section Solid tool is very useful if you are want to create parts which has organic shape to it. The Shell tool on the other hand, is useful to quickly create hollow parts which have constant wall thickness.

To start off, open up a Part Design window in Catia v5. First, create three planes along the x-axis, 3-inch away from each other like so.

Enter Sketch on the original yz-axis and create a 3-inch diameter circle, followed by a 1.2-inch diameter on the second plane, 4-inch diameter circle on the third plane and finally a 2.5-inch diameter circle on the last plane. Ensure that all of the circle are centered at the origin for simplicity purposes.

Now enter Sketch on the first sketch that was create earlier and create two points along the circle using the Point by Clicking tool. Make sure that the points are align with the the zx-axis (It doesn't which axis the points are aligned with. You just have to make sure that future points created are aligned with the same axis that you have used for the first circle).

Now do the same for the other circles too. These points will be used as an anchors for the guidelines that will be used by the Multi-section Solid tool later.

Once you have create the points on all of the circles, enter Sketch on the zx-axis. Select the Spline tool and create a spline with four points above the circles. Next, use the Constraints Defined in Dialog box tool to coincide the points as labeled in the image below (Point 1 with point 1, point 2 with point 2 and so on).

After you are done with that, exit the workbench and re-enter Sketch on the same axis. Create another spline below the circles and repeat the same steps with coinciding the points from the spline to the circles. What you have now is a wire-frame for creating a Multi-section Solid of your vase.

Select the Multi-section Solid tool and a Multi-section Solid Definition window will appear. You will see two white boxes. In the top box, you will want to select the four circles. After selecting the four circles, make sure that the red arrows (circled in yellow) are pointing in the same direction. This step is very important. If the red arrows are not pointing in the same direction, you will be getting a loft operator error message.

In the second box, select the two splines as the guides for this Multi-section Solid. In order to access the second box, just click anywhere on the white space within the second box.

You can now either click Preview to view the outcome before accepting the Multi-section Solid or click OK to just accept the outcome.

You have now created your vase. However, what use is a vase if you cannot put things in it? To create the hollow area in the vase, all you need to do is use the Shell tool. Select the Shell tool and in the Shell Definition window, select the surface at the mouth of the vase as the Faces to Remove.

You can set the Default inside thickness and Default outside thickness to any measurement that you desire. For the purpose of this tutorial, I set the Default inside thickness to 0.05-inch and left the Default outside thickness as 0-inch. Once that you are done, just click the OK button and your vase is finally completed.

I hope that you found something useful in this tutorial. Make sure to check back for future updates in Catia v5 Tutorial for Beginners.

Catia v5 Tutorial: Rib and Slot

2012-06-26T19:50:00.000-04:00

In this post, we are going to cover the Rib and Slot tools. Two quite simple tools.

Say that you want to create a cylinder. There are many ways to create one. One way is to create a circle and pad it. The other way is to create an oblong and fillet the corners. One way would be easier and faster than the other depending on the circumstances. However what if you want to create a cylinder which curves and bend around like in the image below?

In this case, you can make use of the Rib tool. First of all, get into Sketch mode on the yz plane and sketch an outline of the bend.

Next, create the Corners on the edges.

Now, Exit Workbench and create a plane using the Plane tool. In the Plane Definition window, select Parallel Through Point from the drop down menu next to the Plane Type. Select the xy plane as the Reference and select the point which is circled in red as the Point.

If you selected the correct reference and point, the plane should be oriented as shown below.

Enter Sketch on the newly create plane. There, draw a circle of 1-inch diameter with its center coincide with the point which was earlier circled in red. Next exit the workbench and select the Rib tool. In the Rib Definition window, select the circle as the Profile and the bends as the Center curve.

There you have it. You have already created your first part using the Rib tool.

The Slot tool is comparable to the Pocket tool just like how the Rib tool is similar to the Pad tool .

Using the just the circle and the bend that you have created earlier, you can use the Slot tool to remove parts away from a solid. On your Specification Tree select the Rib and delete it.

You will now be left with the circle and the bend that you had created earlier. Now enter Sketch on the yz plane and create a rectangle just as shown below.

Exit the workbench and Pad the rectangle to 1-inch thickness. The pad direction does not matter but if want to have the same orientation as in the image below, just click the Reverse Direction button in the Pad Definition window.

Now, select the Slot tool and repeat the steps that you have taken for creating the Rib. Under the Slot Definition window, select the circle as the Profile and the bend as the Center Curve. This is how your final part should look like:

If your part does not look like in the image above, you can adjust the size of the rectangle used to create the pad so that the Slot will fit nicely within the Pad.

I hope that you found something useful in this tutorial. Make sure to check back for future updates in Catia v5 Tutorial for Beginners.

Catia v5 Tutorial: Shaft and Hole

2012-06-25T20:12:00.001-04:00

It has been quite a long time since my last post. In fact, it has been two years. Anyway, I am back and I hope to pick up from where I left off from the last post.

Instead of making a continuation of the last project, I have decided to start anew. Therefore, this post will be on getting familiar with the Shaft and the Hole tool.

In this Catia project, we will be aiming to create something similar to this part:

Open up Part Design and let's name this part as Bearing Socket.

First of all, we will create a sphere with a diameter of 4-inch. In order to do that, click the Sketch tool and select the yz plane. In the workbench, select the Arc tool which is located in the extension under the Circle tool.

Now draw half a circle and close the arc with a straight line like so:

Exit the workbench and select the drawing that you have just done. Select the Shaft tool and a Shaft Definition window will pop-up. Under axis selection, select the vertical straight line of the half-circle and then click "OK". A sphere should have been created.

Next, click the Sketch tool and select the xy plane. Draw a circle with a 2-inch diameter right next to the sphere that you had previously created. This circle can be drawn anywhere on the screen but preferably somewhere nearby the sphere. Now click the dot at the center of the circle and while holding on to the "Ctrl" button on your keyboard, select any surface of the sphere. Holding down the "Ctrl" button allows you to select multiple elements.

Select the Constraints Defined in Dialog Box tool and select Coincidence. This will automatically align the center of the circle to be coincident with the center of the sphere.

Exit the workbench and click the Pad function. Select the circle and in the Pad Definition window, change the Type to Up to Next and hit OK.

Create a 4-inch Edge Fillet at the edge at the joint connecting the cylinder and the sphere.

Enter sketcher mode on the xy plane again. Create a 5-inch by 2.2-inch rectangle. Use the Contraint tool to align the rectangle as shown in this picture:

Exit the sketcher mode and select the Pocket tool. Under the Type in the Pocket Definition window, select Up to Last, click the Reverse Side button and click OK. You will end up with a part which looks like this:

Click the Hole tool and select the edge highlighted in red, followed by the surface which is labeled as "A".

A Hole Definition window will appear. Under the Extension tab, select Up to Last and set the diameter to 2-inch. This is what your part should look like:

Get into Sketch in the xy plane and draw a hexagon with a diameter of 3-inch.

Select the dotted circle around the hexagon and the circle of the cylinder at the same time. Select the Constraints Defined in Dialog Box tool and select Concentricity.

Exit the workbench and select the Pad tool. In the Pad Definition window, set the Length to 1-inch.

Select the Hole tool and select the bottom surface of the hexagon. In the Hole Definition window, select Blind and set the Diameter to 1.5-inch while the Depth to 3-inch. Next, under the Type tab, select the Counterbore option. Set the Diameter to 1.7-inch and Depth to 0.3-inch.

This is how the inside should look like:

And our simple bearing socket it finally done. This picture will show the 3-view picture of the bearing socket that we have just created.

I hope that you found something useful in this tutorial. Make sure to check back for future updates in Catia v5 Tutorial for Beginners.

Catia v5 Tutorial: Lumber Axe - Part 1

2010-07-19T02:15:00.012-04:00

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

2010-07-17T03:57:00.023-04:00

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

2010-07-16T05:25:00.025-04:00

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.

Welcome to Catia v5 Tutorial for Beginners

2010-07-15T23:16:00.005-04:00

Having trouble with Catia v5?

Got the software but do not know where to get started?

Well, you have come to the right place. Feel free to browse through the blog as I post more tutorials on how to use Catia v5.

I hope that it will help you get familiar with Catia v5.