CATIA V5 Tutorial

Yamaha YZR-M1 2002-2012

2012-03-29T12:30:00.001+08:00

Although it's not a tutorial video I just want to share this video admire these incredible machines. The beauty of the design and the engineering behind the look and performance.

CATIA V5 Bottle Mold Design

2011-10-24T21:48:00.000+08:00

To celebrate my birthday and receiving 100000th visitor today. I will spend my time writing this tutorial that I promised a long time ago. Today I will try to create a 2 parts mold of bottle for plastic blow molding process. I will use the same bottle that was made in the last tutorial.

The first thing we'll going to do is to create a new PRODUCT.
Go the the Core & Cavity Design Workbench (Start > Mechanical Design > Core & Cavity Design).
This will create a new part in the created product.

Import the bottle part from the last tutorial using the Import Model function (Insert > Models > Import).
Choose the xy-plane as reference and use 1.02 expansion ratio.

The imported part will be 2 percent larger than the original.

Then go to the Generative Shape Design Workbench (Start > Shape > Generative Shape Design).
Change the color of the bottle shape (Scaling.1) in the Product tree to other color than the standard color.

Next, use the Extract tool on the Operations Toolbar (or Insert > Operations > Extract) to create only outer surface. Use Tangent continuity in the Extract dialogue box and select the outer surface of the bottle. This step need to be repeated to include the bottle thread surface.

Then Join (Insert > Operations > Join) all the newly created surfaces to make it 1 surface.

After completed the Join process. We are going to split the surface profile into 2 parts. Use the Split function (Next to the Join button in the Operations Toolbar or Insert > Operations > Split. Use the following parameters in the Split Operation dialog box.

Then create new planes using on the bottle opening just as shown in the picture. Use Create new planes feature. Firstly I made a plane on normal to the bottle opening curve. Then created a line to be an axis when making the second plane which is normal to the first plane.

Then by using the Skether tool on the second plane. Create a box as shown in the picture.

Then use Fill function to create a surface from the profile.

Then create some other surfaces surrounding the bottle surface.

Make a half circle using the following parameters.

Then cut the rectangular surface using the circle.

Now Join all the surfaces together.

Now we fill all the space with the Close Surface function.

The completed half-mold.

*NOTE:
In the end I finally realized this product cannot be made as a complete part because I had made a crucial mistake at the start. I should have inserted a Geometrical Set and create all the shapes and surfaces on in instead of importing the original part only.

Unique Shaped Bottle in CATIA V5

2011-03-23T04:32:00.000+08:00

I've been thinking of writing about making a product mold but I was so out of ideas of what product should I design. Finally I decided to make a mold for a bottle. Before a mold can be made we will need a bottle. In this tutorial I will only show you how I made the bottle modeled from a Head & Shoulders shampoo bottle.

The bottle should have 2 parts which is the body and the cap but I just skip the cap part and model only the body. The first step is to go to the Part Design Workbench and make a sketch using the Sketcher Workbench. My sketch is as shown in the picture.

From this sketch I create a Pad with the height of 155mm. I won't be writing too detailed here so if you can't catch up on how I make the sketch or the Pad you may refer to my other tutorials.

After making the pad, I cut some shapes using the Pocket tool. before that we need to sketch the shape to be removed.

In the Pocket Definition box, select the Reverse Direction and make sure the pocket cut through both direction.

Then cut some more shapes using the same methods. This is the sketch.

This is the pocket.

I tried to make an angled cut so I created some planes. The first plane:

The second plane where the sketch will be made on.

Then I made a sketch for the cut.

The use the pocket tool to make the cut.

Then I add a cap holder part to the shape using the Pad tool and add some finishing touch using chamfers and fillets. You may use your creativity on how and where to add the fillets. My end product is like this:

Select the upper surface of the cap holder part of the cylindrical shape. Use the Shell tool and set the Inside Thickness to 2mm. The outer thickness in 0.

Then try to add the cap thread using the Helix tool in the Generative Shape Workbench. (Start > Shape > Generative Shape). To make the thread/spring using Helix tool will require a Starting Point and an Axis. The Starting Point is shown here:

Then to make the Axis I created 2 points and then make a Line from the 2 points.

When the Starting Point and the Axis Line is ready, use the Helix tool to make the thread.

When the helix is ready, create a new plane normal to the helix curve.

On the new plane create a circle of 0.5 mm radius. Then in the Part Design Workbench, use the Rib tool with the Circle as Profile and the Helix as the Center Curve. Now the thread is ready.

Then I add Plastic as the Material and change the rendering properties a little bit. The final product is as shown.

Next tutorial is about how to make a mold for this bottle.

60000 Visitors After 3 Years

2011-02-13T06:33:00.002+08:00

This is just a quick post to announce that on CATIA V5 Tutorial had received it's 60000th visitors on 3rd February 2011. This blog has also been alive for more that 2 years and will reach it's 3rd birthday this July. I'm sorry for the lack of post but I am currently working on a model for writing a new tutorial and I will try to post about it in the next few weeks. I need to successfully make the model before writing about it. Thank you for your support.

CATIA V5R20 SP4

2010-12-29T01:32:00.000+08:00

Image property of Dassault Systemes

I don't realize that the latest version of CATIA V5R20 has been release early this year. It is already end of the year and probably CATIA V5R21 will be released soon. For V5R20, the latest update available currently is Service Pack 4 (SP4). Here I just want to share something about R20.

CATIA V5R20 includes new innovations such as:

CATIA ICEM Shape Design (ISD) - ISD R20 extend the advanced and powerful freeform surface creation, modification, and analysis capability within the Automotive Class A modeling domain.

Composite data in STEP format - Allow long term archiving of composite data especially for the aerospace industry. This function leverages the exchange of data between different CAD vendors. Users can greatly increase productivity with Light Manufacturing Part Generation which ensures that manufactured parts can be quickly created and synchronized with designed parts.

Imagine and Shape - For industrial designers, this function combines the curve-based approach with subdivision surfaces clay modeling. Beneficial to the styling centers/design studios transportation and product design industries.

Functional Modeling Part - Enhanced to address design processes of customers in powertrain domain as well as to support complex part design. Functional Modeling allows users to design oil pans, gear boxes, or motor brackets up to 40% faster.

CATIA 2D Layout for 3D Design - Allow users to cut a part along multiple planes. Then users can instantly visualize several internal features such as holes or slots in a single view to better understand the geometry and annotations.

SIMULIA Rule based Meshing - Automate the process of creating high quality surface meshing for all workflows that use CATIA meshing tools.

Information from Dassault Systemes: CATIA V5R20 Portfolio

Modeling Fan or Propeller Blades

2010-12-09T03:25:00.001+08:00

Fan or propeller blades are aerodynamic shapes. To have a functional fan or propeller blades you will need to do some calculations or you might already have the data configured for your projects. In this tutorial I will only create a shape from my imagination without a proper dimension. Here's where I'll start:

Start your CATIA program and go to the Part Design workbench (Start > Mechanical Design > Part Design). I will start by creating the hub for the blades to be connected to. Select the zx-plane and start the Sketcher workbench. Draw something like I draw in the 1st picture.

After finishing creating the Sketch.1, exit the Sketcher workbench and you will notice the Sketch.1 link in the design tree. Select the Sketch.1 and click the create Shaft icon or Insert > Sketch-based features > Shaft. Then select the x-axis as the rotation axis. Press OK and the hub will be created.

Now I want to create a drill hole at the center of the hub. Select the front flat surface and click on the Hole icon on the toolbars or Insert > Sketch-based Features > Hole. In the Hole Definition box, select Up to Last for the hole extension type, set the diameter to be 20mm and maybe Countersunk for the hole type. Press OK when you satisfied with the hole.

Then go to the Generative Shape Design Workbench (Start > Shape > Generative Shape Design). Create a new plane using the xy-plane as reference. Set the offset to be around 40mm. After done creating the new plane. Select the plane and click on the Sketcher tool. We are going to make a new sketch on this plane. In the Sketcher workbench, create the starting shape for your propeller blade using the Spline tool. If you want to create a real propeller blade you might need to create points based on your propeller dimension and then connect the points. I just made up the shapes as shown in the next picture.

When you exit the Sketcher workbench it will look like this:

Repeat the steps (creating planes and profiles) with different profile shapes to look like a propeller blade. Mine look like shown in the next picture:

Now in the Surfaces toolbar, select the Multi-Sections Surface tool. (Insert > Surfaces > Multi-Sections Surface). Then when the Multi-Section Surface box appeared. Select all the profiles you have just created. Press the preview button and it will look a bit weird. Don't worry about that. Create the profiles properly next time. In the Coupling tab in the definition box select Tangency for the Sections Coupling. Press OK when done.

Then select the last profile/sketch you've created (mine is Sketch.10). Click the Fill tool on the Surfaces toolbar. When the Fill Definition box appeared. Sketch.10 will appear for the curves. Click on the Multi-Section surface we created before and it will then become the support for the Fill. Set the Fill Continuity as Tangent. Press OK when done and the fill will be a continuation of the Multi-section surface.

Then use the Join tool on the Operations toolbar (Insert > Operations > Join) for the Fill and Multi-Section Surface to make them become 1 entity.

To make things easier, hide everything except those we created in the Part Design Workbench and the Join.1. The go back to the Part Design Workbench. Click on the Close Surface tool, Insert > Surface-based Features > Closed Surface. Then select the Join.1 entity as the object to close. Then press OK.

The Close Surface and Join.1 is now at the same location. Next hide the Join.1 and let only the CloseSurface.1 to be visible. A blade is now created. Next use the Circular Pattern (Insert > Transformation Features > Circular Pattern) to multiply the blade. The Circular Pattern definition box will appear. In the Axial Reference tab, select Complete Crown for the Parameters, select any circular or cylindrical surface for the Reference Direction > Reference Element, and Instance(s) to be 4, 5 or any amount you like. Done. You blades have been created.

A video for this will be uploaded when I have access to faster internet connection.

Modeling a Formula 1 Front Wing in CATIA

2010-03-28T09:40:00.001+08:00

I received a lot of request from friends to teach them about surface modeling in CATIA V5. In this tutorial I will demonstrate how to use the Generative Shape Design workbench to create an F1 front wing. I will not make it in real scale as I don't have any dimension with me.

Start the workbench by selecting Start > Shape> Generative Shape Design. A dialogue box will appear for you to name your part. Rename the part as F1FrontWing or any name you want and click the OK button. Then your part will be created and you are now in the Generative Shape Design workbench.

Select the yz-plane and click on the Sketcher Tool icon. In the Sketcher workbench create a drawing of dimensions as shown in the figure below:

Once the drawing has been created, go back to the Generative Shape Design workbench. Create a plane using the Insert Plane icon or select Insert > Wireframe > Plane. In the Plane Definition box select Offset from plane for the Plane type, yz-plane as the Reference plane, and 100mm Offset as shown in the figure:

Now you have a new plane. To make things simple, we will copy the previous drawing and paste it on the new frame. To do this, double-click on the Sketch.1 in the design tree to open the 1st drawing in the Sketcher workbench. Select all the lines and curves and copy them (ctrl+c). Then exit the Sketcher workbench, select the new plane you had just created, click on the Sketcher tool icon, and paste (ctrl+v) on it. After the drawing had been pasted, what we will do next is to resize all the dimensions to half of their current values. Note that while doing this the 1st drawing also appears in the background so it is advisable for you to hide it. See the next figure:

After done with the second drawing, exit the Sketcher workbench. Now you should have 2 profiles.

Next is to fill in some shape to the profiles. I will not make this as beautiful as a regular F1 wing look like. First is to connect both profiles together and create the basic shape. I will use the Blend tool for this. The Blend tool is on the Surface toolbar. Select the Blend tool and in the Blend Definition box, select the first sketch (Sketch.1) for First curve and Sketch.2 for Second curve. Then press Preview to take a look at the generated shape and press OK when you are satisfied.

Now we shall close the front hole using the Fill tool which is also on the Surface toolbar. In the Fill Definition box select Sketch.2 for Curves and Blend.1 for Support, and select Tangent for Continuity. Then press Preview. The fill is now generated. Try change the Continuity to Point and press Preview and you will see what is meant by Continuity.

We will need to combine these two surfaces by using the Join tool which is on the Operations toolbar or you can select Insert > Operations > Join. In the Join Definition box select Blend.1 and Fill.1 as the Elements To Join and press OK. After joining them together, the Blend.1 and Fill.1 is now combined to be 1 surface of Join.1.

You can now hide Sketch.1 and Sketch.2 before we go to the next step. What we have created is a shape. The problem for some people is that they know how to create such shapes but didn't know how to convert them into parts like those you created using Part Design Workbench. To create a part out of this shape, we will need to go to the Part Design Workbench. Select Start > Mechanical Design > Part Design. Make sure you are not creating a new part but still using the same part in different workbench. Click on the Thick Surface tool or select Insert > Surface-Based Features > Thick Surface. In the ThickSurface Definition box, select Join.1 as the Object to offset, set the First Offset to be 2mm and Second Offset to be 1mm. Press Preview to see the changes. After pressing OK, a part is created base on the shape you had designed. You can now hide Join.1.

What we have created is just the nose. Now go back to the Generative Shape Design workbench to create the wing. Create a plane using the Create Plane tool then in the Plane Definition box select Plane Type to be Tangent to Surface. For the Surface and Point, select the face and point as shown in the figure below. Click Preview then drag the point to about the center of the face before pressing OK.

Select the new plane and click on the Sketcher tool. Draw an curve using the Spline tool.

Now create another plane. In the Plane Definition box, select the Plane Type to be Offset from plane. Select the zx-plane to be the Reference plane and the Offset to be 150mm.

In the design tree you will see the new plane is named Plane.3. Select this plane and click on the Sketcher tool. Then create another curve as similar to the one you draw prevously but with smaller dimension as shown in the figure:

Then create another plane similar to Plane.3 but this time the Reference plane is Plane.3. The Offset is still 150mm.

Create another curve profile but smaller that the second curve

After you exit the Sketcher workbench there will be 3 curve profiles.

Next we are going to create a shape out of the 3 profiles using Multi-Sections Surface tool in the Surface toolbar. In the Multi-Sections Surface Definition box, select the 3 curve profiles (Sketch.3, Sketch.4 and Sketch.5). Before pressing Preview, check the arrows that appeared on each profiles. They all should be on the same direction or the shape cannot be generated. Click on arrows that is pointing the other direction to change its direction. Once all the arrows are pointing in the same direction, press the Preview button. If your shape is generated and no error message appeared then press OK.

To make it look better I will add another layer of surface for the wing similar method as before.

Next we are going to make plates out of these wing shapes. Go to the Part Design Workbench and use the Thick Profile tool just as we did previously. Set the 1st Offset to be 1mm while 2nd Offset to be 0mm. For the second plate, set the 1st Offset to be 0mm and 2nd Offset to be 1mm. This is to prevent the two wing plates from being joined together.

To add some pretty finish to the wing. Create a plane 300mm Offset from the zx-plane. Then make something like in the figure using Sketcher and Pad.

When I try to Mirror this part a problem occured because the nose is a complete part. To solve this we need to cut the nose into half. The task is to use the Pocket tool. Select the yz-plane and create a big box to cut the nose part using the Pocket tool.

Next is to Mirror the part using the Mirror tool and select the zx-plane the Mirroring element.

CATIA V5 Tutorial Reached 20000 Visits

2010-02-16T21:46:00.000+08:00

I would like to express my appreciation for all of you who visit and read this blog. CATIA V5 Tutorial had received its 20000th visitors today since the launch in June 2008. It is not a big figure since this blog reader only started to increase since the middle on 2009. I do hope there will be more visits from now on. I am also very sorry that I could not update this blog frequently because of my work. I hope what is contained in this blog might had helped you in some way.

I would also like some suggestion from reader on topics or tutorial that I should write in this blog or any other suggestions. You can also comment on the blog appearance, loading speed, contents or navigation. I'll be waiting for some feedbacks from you. Thanks again for visiting and reading CATIA V5 Tutorial.

Modeling Universal Joint in CATIA V5

2009-11-22T03:51:00.009+08:00

Hi.. Today I'm trying to model a simple universal joint and I hope everything will work fine as intended. There are no complex shapes involved therefore I'm only using the Assembly Design and Part Design Workbench. The DMU Kinematic Workbench might be used to model the simulation.

The first step is to enter the Assembly Design Workbench and create a new product. Rename the product from Product1 to Universal Joint. Then by right-click on the product name, select Components > New Part. Rename the new part as Shaft. By double-clicking on the new part name you'll be redirected to the Part Design Workbench to model the first part.

In the Part Design Workbench, select the yz-plane and click on the Sketcher Tool icon (or Insert > Sketcher > Sketch). In the Sketcher Workbench, create something as shown the the figure below:

Then elongate the part with a 40mm diameter cylindrical shaft of about 300mm length. Then some make-ups with fillets will make the part look a little nicer. Create a 10mm diameter hole to insert the connector to the shaft as shown in the figure. Finish the part with more fillets.

Then double-click on the Universal Joint product to go back to the Assembly Design Workbench. Similar to the first step, insert a new part to the product and rename it as Connector (or anything else as you like). Double-Click on the Connector to model it in the Part Design Workbench.

Create a T-cross with 10mm diameter to fit the hole of the shaft and 80mm length.

Back in the Assembly Design Workbench, duplicate the Shaft part by using the Fast Multi Instantiation function (Ctrl+D or Select the Shaft part and select Insert > Fast Multi Instantiation). Use the Manipulation tool to move the part to a proper location. Assemble the Shaft parts with the Connector part using the Coincidence Constraints.

The Shafts and Connectors are rotating parts therefore we need a fixed part to anchor the shafts. Create another part to be a base for the shafts to rotate. I made a couple of blocks with 40mm groove to be assembled with the shafts. The blocks are distanced by 150 degrees angle.

After completing the blocks, fix the blocks using the Fix constraint and assemble them with the shafts using the Coincidence Constraint and try use the Manipulation tool to check if the assembly is correct. Check whether all the parts are moving as intended when the "With respect to constraints" are ticked.

Kinematic Simulation Demo Video

2009-10-08T16:32:00.002+08:00

Hi guys.. Sorry that I don't write a new update for this blog because I still can't spare some time to write a new tutorial. Last night I helped my friend with his robotic project and while at it I've recorded a video to show him how to make a kinematic simulation. Hope you guys can take a look at the video. It is just a rough demo without any detail explanation. I'll provide a written tutorial related to that simulation later. Please wait and thank you for your attention.

Modeling a Simple Heat Exchanger - Continued

2009-05-23T17:39:00.014+08:00

A heat exchanger will require at least 2 medium for heat transfer. For this model, the medium are 2 fluids. 1 is flowing through the spiral tube and another fluid flows outside the spiral tube in a closed chamber. Now we are going to make the chamber. Last time we stop was after modeling the spiral tube. As seen in the picture, I've set copper for the material property and adjusted

the rendering.

Now right click on the Parent tree and create a new part. Name the new part as Chamber. After a new part has been created, activate the Chamber design by double click on it and go to the Generative Shape Workbench (Start > Shape > Generative Shape Design). Make sure you are not creating a new part that is not in connection with the Heat Exchanger. If a Create New Part dialogue appeared, closed it reactivate the Chamber Part Tree.

In my version, both Spiral Tube and Chamber shares the same origin. I dont want to change this because it will be helpful during the modelling of the chamber. By selecting the yz-plane, activate the Sketcher Workbench. Create a circle of slightly larger than the diameter of the spiral tube. I set is as 85 mm.

What to do next is to create more circles like this at other location and join them. Length of the helix was 200mm therefore i'll create another circle of similar dimension 200m apart respective to the yz-plane. Some additional planes are required to make those circles. For the 35mm diameter circle, the plane is 30mm from the yz-plane and the 28mm diameter circle is 20mm from the 35mm circle.

Then you should have something like this.

Then we are going to make a surface from these circles. Select the Multi-Section Surface tool (Insert > Surfaces > Multi-Section Surface) and select all 6 circles. Press Preview to view the generated surface.

Done with that, we will have to generate solid part from the surface. For this, we will have to go to the Part Design Workbench. Select Start > Mechanical Design > Part Design without changing anything. Select the Thick Surface tool (or Insert > Surface-Based Features > Thick Surface) and select the generated Multi-Section Surface. Set the first offset to be 2mm that will make the solid generated outward and press OK. Now the Chamber complete.

There are several holes needed to fit in the Spiral Tube but maybe you can do them later. Apply Steel material to the Chamber part and adjust the rendering property.

Modeling a Simple Heat Exchanger

2009-04-25T17:27:00.006+08:00

Mechanical Design > Part Design
Shape > Generative Shape Design

This tutorial is to model a simple heat exchanger consist of a chamber and a spiral tube. I'm trying to analyze the heat extraction capability of this and other models for my research project of extracting wasted heat from automotive exhaust. I'll continue the automotive engine design later.. very sorry about that.

The first step is of course starting the CATIA software. By default, a product tree is opened automatically in the Assembly Design Workbench. Rename the product as Heat Exchanger. Then insert a new part into the product (right-click > Components > New Part) and name the new part as Spiral Tube.

Double-click on the PartBody of the Spiral Tube to activate the Part Design Workbench. The spiral tube is to be made from a helix therefore we'll have to use the Generative Shape Design Workbench. By keeping the Spiral Tube part selected (highlighted), select Start > Shape > Generative Shape Design. Now create a helix with starting point = (0,0,30)mm, rotation axis = x axis, pitch = 20mm, height = 200mm and left other values as default. Refer Modelling a Spring in CATIA on how to make the helix.

Now we'll create 2 lines to be connected to each end of the helix. Select the end-point of the helix at (0,0,30) coordinate or the starting point of the helix. By using the line tool, create a line of 100mm as defined in the figure.

Then do the same thing to the other end of the helix. Done with that, we'll have to join the helix and the 2 lines together and remove the corner before we can sweep the curves into a tube. To join them, use the Join tool in the Operations toolbar (or Insert > Operations > Join). Select the helix and lines for Elements to Join in the Join Definition Box. If the join is successful, the helix and lines will now be a single part. You can check in the PartBody tree.

To remove the corner, we'll use the Curve Smooth tool. In the Curve Smooth Definition box, select Join.1 for he Curve to join, set 10mm as the Maximum Deviation, and select Curvature as the Continuity type. After accepting the values, the corners will automatically be converted into curves.

Done with the curves, go to the Part Design Workbench and create a plane at 1 end of the curves and normal to it. Check the figure.

Then by selecting the new plane, draw some circles to be the inner and outer diameter of the tube. Make the outer diameter as 20mm and inner as 18mm. If somehow you get confused on where to place the center of the circles, while in the Sketcher Workbench, pan the view so that you can have a 3D look on where the end of the curve is. Then select both the end point of the curve and the center point of the circle and Coincidence them together.

Then exit the Sketcher Workbench and back to the Part Design Workbench. Make a Rib and select Sketch.1 for the profile and Curve smooth.1 for the center curve. After pressing OK, you'll have the Spiral Tube part. Apply Copper as Material and save the file.

To be Continued..

Welding Design in CATIA

2009-03-29T23:41:00.012+08:00

Mechanical Design > Weld Design

This tutorial is about making weld joint in CATIA Weld Design Workbench.

Go to the Weld Design Workbench (Start > Mechanical Design > Weld Design). Rename the product as Welding Demo. Right click on the product tree and create a new part (Right-click > Components > New Part). After the new part has been created, expand the part tree and double-click on the part name to go to the Part Design Workbench as shown in the figure.

In the Part Design Workbench, create a rectangular bar of 100x50x10 mm dimension. Check my other blog entry if you don't know how to create the bar.

After finishing the bar or plate, double-click on the Welding Demo main product tree. This will automatically brings you back to the Weld Design Workbench.

Now make another part just by copying the existing part. Right-click on the Part1 (Part1.1) instance and select Copy Instance. Then click on the Welding Demo parent tree. Automatically Part1 (Part1.2) will be created under the existing part in the tree.

The new part is exactly at the same position with the previous part. Use the manipulation tool or the compass to position them apart of each other.

The weld function is different than the assembly feature because you'll have to position the part correctly in order to successfully make the weld join. If the parts are not in the correct position, you'll be receiving error messages every time you want to make a joint.

The first step is to assemble them using constraints. We'll use coincidence constraint to connect edges of the part before making the weld joint. Select the coincidence constraint and select edge 1 and 2 as shown in the figure below. Then create another coincidence constraint and connect edge 3 and 4 together.

After pressing the update button, the parts should connect together as shown.

At this point, you still can't make a weld joint because some surfaces required as joint parameters are hidden after being constrained. A little trick is required here. First, fix the first part with the Fix Component constraint. Then expand the Constraints tree and deactivate constraint 2 (coincidence.2) that connects edge 3 and 4. Don't delete it. Then use the manipulation tool with the "with respect to constraints" is checked to move part 2 in the x direction just like as shown in the figure.

Now select the Single V-Butt Weld feature or Insert > V Butt Welds > Single V-Butt Weld. A box will appear for you to adjust the welding parameters. Change the height to 5mm, shape to convex with 0.5mm offset, and select surfaces as numbered in the figure above respectively. You can click on the Selection Assistant to help you select the surface in order. Press Enter or OK button to make your weld joint.

After that, reactivate constraint 2 (coincidence.2) and press the Update button, the parts will repositioned as before and you now have your weld joint.

Automotive Engine In CATIA 1 - Calculations

2009-03-11T21:50:00.001+08:00

Mechanical Design > Part Design

I'm showing how to model an automotive engine in CATIA and to measure some of it's properties. For this entry, I'm writing about all the basic parameters required to model a working automotive engine. Later I'll write about modeling other automotive engine parts and show how to assemble them and make a kinematic simulation.

To make a valid and functional assembly, all parts need to have correct dimensions that will fit to each others. Therefore every dimension has to be measured, calculated and recorded. I don't have any actual model with me therefore I'm going to make all other parts based on the engine displacement. All dimensions for the parts are just made up based on calculations from the engine capacity.

Measuring the Bore and Stroke:

I'm going to make a short-stroke, high-rev V8 engine with oversquare piston just like a racing engine. The engine capacity is 2.4 liter like the F1 engine. Some calculations is required:

Assuming an F1 engine with 19000 rpm maximum revolution would have Stroke length of 39.77 mm.

Engine capacity = 2.4 liter = 2400 cm^3

V = N*(π/4)*(B^2)*S

V = Total engine capacity
N = Number of cylinders
B = Bore size
S = Stroke length

B = [(4/π)*(V/N*S)]^(1/2) = [(4/π)*(2400cm^3/8*3.977cm)]^(1/2) = 98.0 cm

Therefore the Bore size is 98.0 mm

Measuring the Crank Offset and Connecting Rod Length:

These parameters are required at early stage because the length of the pistons depend on the crank offset (crank circulating radius) and the connecting rod length. The engine should be compact to reduce space and to have low center of gravity. Piston size will influence the overall engine dimension.

Distance between crank axis and piston pin axis is:

s = a cos θ + (r^2 - a^2 sin^2 θ)^(1/2)

a = crankshaft offset
r = connecting rod length
θ = crank angle measured from cylinder centerline.

When piston at TDC, θ = 0°

Therefore:

s = a + r

Stroke = 2 * crank offset
S = 2a

a = S/2 = 39.77 mm/2 = 19.89 mm

Assuming the engine to have connecting rod length to crank offset ratio, R = 5.13
(R ranges from 2 for small engines to 10 for large engines)

R = r/a

R = Ratio of connecting rod length to crank offset
r = connecting rod length
a = crank offset

r = aR = 19.89 mm * 5.13 = 102.04 mm

s = a + r = 19.89 mm + 102.04 mm = 121.93 mm

*Note the use of capital S and small s

V-Block Configuration Angle and Bore Spacing

A complete 4-stroke cycle requires 720° revolution. For a V8 engine, the best angle is:

720°/8 = 90°

For this angle, spark firing occurs at every 90° rotation of the crankshaft. This angle provide the best firing sequence that help to reduce vibration. Other angles are possible but mostly requires adjustment to the firing order and timing in order to balance the engine. There is also a need for balancing shaft to reduce vibration.

Crankshaft Configuration

Common V8 engines use crossplane crankshaft where the first and last of the four crank pins are at 180° with respect to each other as are the second and third, with each pair at 90° to the other, so that viewed from the end the crankshaft forms a cross. The cross-plane can achieve very good balance but requires heavy counterweights on the crankshaft. This makes the cross-plane V8 a slow-revving engine that cannot speed up or slow down very quickly compared to other designs, because of the greater rotating mass. However, racing engines usually use flatplane crankshaft where the crank pins are at 180°. Flatplane crankshaft does not require counterweights therefore having less mass and inertia and allow higher speed and acceleration. Flatplane crankshaft are imperfectly balanced and thus produce vibrations unless balance shafts are used, with a counter rotating pair flanking the crankshaft to counter second order vibration transverse to the crankshaft centerline. I'm still looking if this engine we're going to build will require a balancing shaft or not.

*This post will be updated when further calculations are required.

CATIA V5R19 Works With Windows 7

2009-02-18T02:49:00.002+08:00

Dassault Systemes claimed that CATIA V5R19 is fully compatible with Windows Vista. This should mean that it is compatible with both 32bit or 64bit operating systems. A discussion from Overclock.net stated that CATIA V5R19 is also operatable in Windows 7 64bit beta. Further details for this statement is not available to clarify on which service pack was tested.

New features in R19 are the In-Context Composite Design that could optimize the composition of large composite parts for mating sub-stuctures. R19 also features CATIA Imagine & Shape Workbench for fast surface creation from curves. The best features that we had always been waiting for is the ability to support new file formats such as Solidworks SW2007, SW2008, SolidEdge V20, Parasolid V18, and Unigraphics NX5 and NX5. With support for these formats, we can easily integrate a Solidwork model into CATIA for analysis or other funtion.

Modelling the RSS Feed Icon

2009-01-22T23:15:00.007+08:00

For this session, I'm going to show you how I made an RSS feed icon in Catia. This is just a simple tutorial made just to update this blog. I hope you can still learn something from this.

Select Start > Mechanical Design > Part Design. Name the new part as RSS Icon.

In the Part Design Workbench, select the yz-plane and click on the Sketcher Tool .

In the Sketcher Workbench, create a rectangle of 70mm x 70mm. Use the Constraint tool to adjust the dimension.

Create 2 lines with 12mm offset from the rectangle lines. The lines intersection will be the center of the circles to be made after this.

In the figure, the 2 lines are dotted meaning that they are construction lines. Use the Construction/Standard Element tool to change any lines to be standard element or construction element.

Then create 4 circles that centered on the two lines intersection. Radius are: 22mm, 31mm, 38mm, 47mm. Use the Quick Trim to remove all the unwanted curves. Don't delete the 2 lines that was made earlier.

Make a circle tangent to both two lines. Set the diameter to be 12.5mm.

Now you can delete all unwanted lines or curves. Make sure that every profile maintain their positions when you are making the trim.

From this section, you can either Pad the sketch in Part Design Workbench and apply Fillet later or apply Fillet now in the sketch before making the pad. To apply fillet (corner) to the rectangle, choose the Corner tool in the Dress-up Features Toolbar and select the lines where you want the cornet to be. Set the corner radius to be 13mm.

After finish applying the corner, exit the Part Design Workbench and Pad the sketch with 20mm thickness. To add some color and shines, specify material for the part using the Apply Material tool . After applying the material, right-click on the material properties to adjust the color and other rendering properties. Your final part should look like the figure below. Thanks for reading. I'll write something more useful when I'm not too busy.

Make a Guitar with CATIA

2008-12-07T02:54:00.015+08:00

Mechanical Design > Assembly Design

Start the Assembly Design Workbench by selecting Start > Mechanical Design > Assembly Design or File > New > Product. Rename the product to Guitar (right-click on Product1 and select Properties).

Create a new part for the product (Right-click on Guitar and select Components > New Part).

Double-click on the yz-plane to switch into the Part Design Workbench.

With the yz-plane selected, click on the Sketch tool to enter the Sketcher Workbench. In the Sketcher Workbench, make a reference line with the Line tool from the origin to about 300 mm length. Then create some shapes to model a guitar by using any tools such as Circle, Splines, etc, on the upper side of the reference line. After that, use the Mirror tool to complete the shape (press ctrl to select many shapes or lines together). After completing the mirror process, convert the reference line to Construction Element and check the sketch with the Sketch Analysis tool from Tools > Sketch Analysis.

Make a Pad with 30 mm thickness in the Part Design Workbench.

Select the front surface and select the Shell tool (Insert > Dress-Up Features > Shell). Set the default inside thickness to 2 mm.

Copy the Sketch.1 drawing under the Pad.1 tree and create another part in the Guitar tree. Double-click on the Guitar tree and create a new part. Then paste the sketch in the Part2 section. You should see a sketch appearing in the PartBody section.

Then double-click on the Guitar parent tree to be in the Assembly Design Workbench. With the Manipulation tool, move the Part2 in front of the Part1 with respect to the x-axis.

Double-click on the Part2 and enter the Part Design Workbench. Select the front surface and enter the Sketcher Workbench. Make an acoustic hole on the surface with 35 mm diameter and with the Pocket tool.

Double-click on the Guitar parent tree and create a new part for the neck and fret. Again select the yz-plane and enter the Part Design Workbench. Use the Sketch tool to draw the neck.

Make a pad of 10 mm thickness from the neck sketch. Apply some dress-up features such as Fillet, Pocket, etc. to make the neck look more realistic.

After some modifications, the neck should look like this.

To make tuner holes, select the Hole tool and make a 2 mm diameter hole. With the Rectangular Pattern tool , make copies of the holes with suitable spacing and reference element.

After that, double-click on the Guitar parent tree to return to the Assembly Design Workbench. In the workbench, use the Manipulation tool and Assembly Constraints tool to place the parts in suitable position. Apply colors or material to make the guitar more beautiful. The guitar is now complete. Later actions are up to u.

CATIA V5R19 with SP2

2008-11-24T01:32:00.001+08:00

I've notice that CATIA V5R19 with SP2 is now available. It must be fully compatible with vista but I don't know whether it is 32bit or 64bit or both and whether it can be installed in 32bit vista or 64bit only.

Ask What You Want

2008-11-24T01:20:00.004+08:00

Hello readers. I can see that some people really using this blog as reference. I'm kind of blur and don't know what to write here and I'm a little busy to write a long post like in this blog.

Please leave comments and ask me what you really need about Catia and I shall help as much as I can.

Bolt & Nut - Threading

2008-11-16T21:58:00.031+08:00

Mechanical Design > Part Design

In this tutorial I'm going to show how to make bolt and nut that will involve threading.

Open the Assembly Design Workbench because we are going to create both bolt and nut and will assemble them together.

In the Workbench, right-click on the Product1 tree and select properties. When the Properties box appeared, rename the Part Number to Bolt&Nut and click OK. You'll see the Product1 name had been changed to Bolt&Nut.

Then right-click on the Bolt&Nut tree and select Components > New Part. As the new part has existed, expand the tree and select the properties of the new part. Rename both the Instance Name and Part Number to Bolt as shown in the figure.

Now double-click on the xy-plane and we'll be automatically switched to the Part Design Workbench. Then select the Sketcher tool to make the first drawing. In the Sketcher Workbench, select the Hexagon tool. (click the arrow below the Rectagle tool to view the Hexagon tool) or select Insert > Profile > Predefined Profile > Hexagon. Then resize the hexagon using the Constraint tool at the circle surrounding the hexagon. Adjust the diameter value int the Constraint Definition box to 30mm.

After done with the hexagon, exit the Sketcher Workbench and make a pad from the Sketch.1 with pad length of 10mm. Make sure u select the Reverse Direction button as shown in the figure.

Done with the pad, select the lower surface of the part as shown in the figure and use the Sketcher tool again. Create a circle at the center of the hexagon with a diameter of 16mm. Then exit the Workbench and make another pad from the Sketch.2 with 50mm pad length.

Now we are going to insert some thread to the bolt. Click on the Thread/Tap tool or select Insert > Dress-up Features > Thread/Tap. A Thread/Tap Definition box will appear and enter values as shown in the figure below.

*Note. The thread will not be visible unless in the Drafting Workbench.

Now we are making the nut.

Right-click on the Bolt&Nut tree and insert New Part. Rename it to Nut.
Create a part with similar method as above except for the second sketch (Sketch.2) the diameter is 15mm and make a pocket instead of a pad. Values for threads are as same as above.

Double click on the Bolt&Nut tree to activate the Assembly Workbench. Use the Manipulation tool to move the nut and bolt together as shown in the figure.

With the Bolt&Nut still selected, select Start > Mechanical Design > Drafting. Just click OK when the New Drawing Creation box appear.

Click on the Front View tool or select Insert > Views > Projections > Front View. Then select the window toolbar and select the Bolt&Nut.CATproduct (switch to the Assembly Workbench view).
Then select a flat surface of the bolt to be the front surface for the drafting. Then rotate it to a suitable view.

Right-click on the properties of the Front View projection and check the Center line, Hidden Lines, Axis, and Thread.

*Note: Thread shown in this view is according to the Standard of CAD Drawings.

Making An Assembly

2008-10-25T20:46:00.063+08:00

Mechanical Design > Assembly Design

In this page, I want to demonstrate how to assemble some automotive parts together. I'm using parts that I've already have so this tutorial is to be a reference on how to make an assembly. You should try again when you really have some parts ready to assemble.

When making assemblies, you should visualize what type of constraints to be used. It is either to use the Coincidence Constraint, Contact Constraint, Offset, Angle, etc.

There is another way where we can create parts while making an assembly but I'll show it later because I'm in a really tight schedule right now.

Start the Assembly Design Workbench by selecting Start > Mechanical Design > Assembly Design or select New > Product which will automatically brings you to the Assembly Design Workbench. (If it's not, try the first step)

In the Assembly Design Workbench, you'll see a product tree on the top left corner with Product1 as the parent. You can change the name by modifying the properties.

Now right click on the Product1 tree and select Components > Existing Components or select Insert > Existing Components or click on the Insert Existing Component Icon .

A File Selection box will appear and select all the parts to be assembled.

Now all parts have been loaded but all at the same place. Just click on the Explode icon on the Move Toolbar . The parts shall be spread automatically.

We start by fixing the crankshaft using the Fix Constraint or select Insert > Fix and then select on the crankshaft on the screen or on the tree.

To assemble the piston and the piston pin, select the Coincidence Constraint . Then select the outer surface of the piston ring and the inner surface of the piston hole. An axis should pop-up on each cylindrical profile you are selecting that will guide you to select the correct profile.

After the Coincidence Constraint had been established, you should notice the Update Button is active and the constraints on the parts are in dark color. After you pressed the Update Button, the constrained parts should automatically moved to follow their constraints. Then you should see that the Update Button is not active anymore and the constraints are in green color indicating that the parts are in their constrained positions.

Now to make the piston pin exactly in the correct position, we have to insert another constraint between the piston pin and the piston. Select the Coincidence Constraint and select surface 1 and 2 as shown in the figure below.

After that, just push the Update Button so that they move to their correct position.

Then connect the connecting rod to the piston pin using the same method as above. Just try and error to obtain what you want. (the Undo function will be very important).

To move any part to any direction, use the Manipulation Function on the Move Toolbar shown above. After you have selected the Manipulation Function, a Manipulation Parameter Box shall appear and make sure you checked the "With respect to constraint" box. With this, the parts will only move according to their constrained positions.

When using the Contact Constraint , you should know which surface to be involved. After each constraint, try using the Manipulation Function with the "With respect to constraints" checked just to make sure the assemblies and constraints are correct. If the parts are moving just like you intended to, it means that the assemblies are correct. If not, try revise your assemblies. Try to remove the Fix constraint on a part and apply it to other part. Then use the Manipulation Function to check how the parts move.

*I'll make a simple assembly tutorial because I don't feel this is quite helpful. Is it?

My Video Tutorials 1

2008-09-05T20:53:00.020+08:00

Video Tutorial 1 > Making a Sketch

I'll show u how to sketch this in CATIA.

Video URL: http://www.youtube.com/watch?v=ltkpKtDALaQ

Video URL: http://www.youtube.com/watch?v=2S54C43VovA

Valve Body

Video URL: http://www.youtube.com/watch?v=9jeXmoc3f-w

CATIA FEA

Video URL: http://www.youtube.com/watch?v=6qR5QBcg80Y

Pulley Housing

Video URL: http://www.youtube.com/watch?v=gjgxPrxdxKU

CATIA Drafting (Pulley Housing)

Video URL: http://www.youtube.com/watch?v=wi1ORSD1EPk

Failed Simulation ;D

Video URL: http://www.youtube.com/watch?v=cKe3N7-hQyE

CATIA V5R18 SP4 On Vista

2008-09-03T20:35:00.007+08:00

News > CATIA V5R18 SP4 On Vista

Great news. CATIA V5R18 SP4 onward can be clean installed in Windows Vista. The version can be installed on both x86 or x64 Vista. Previously I used the R17 version which was installed on WinXP and then Upgraded to Vista because the previous version of CATIA installer won't even run on Vista. Now u can install or uninstall CATIA on Vista without any problem.

**Correction**

The version of CATIA I'm using is 32bit CATIA V5R18 with Service Pack 5 (just installed today). The CATIA version can only be installed in a 64 bit Vista. I dont know about the compatible XP. For Vista 32 bit.. I dont know.. sorry.. tell me if u do. The are Service Pack for 64 bit CATIA R18 but I dont have the 64 bit CATIA version. If Anybody know about CATIA V5r18 64bit version please do tell me.

Modelling a Bottle in CATIA

2008-07-25T23:17:00.035+08:00

Mechanical Design > Part Design

*Note in this page I used CATIA P3 Environment. The functions is same as P2.

Start the Part Design Workbench (Start > Mechanical Design > Part Design). Select the yz-plane and click on the Sketch tool or select Insert > Sketcher > Sketch.

In the Sketcher Workbench, create a Spline to resemble a half-bottle. Alt: Insert > Profile > Spline > Spline. Add some horizontal and vertical lines to complete the half-bottle.
*Note the position of the axis of the plane.

Exit the Sketcher Workbench to get back to the Part Design Workbench. Click on the Shaft tool. In the Shaft Definition box, select Sketch.1 for the Profile/Surface Selection. Right-click in the Axis Selection box and select the z-axis as the axis of rotation.

Now select the top surface of the bottle and click on the Shell tool. Alt: Insert > Dress-Up Features > Shell. In the Shell Definition box, enter the values as shown below. (Default inside thickness = 1mm, Default outside thickness = 1mm, Faces to remove = Shaft.1\Face.1, Other thickness faces = No Selection)

Now we have a bottle. Good Luck.

Modelling a Spring in CATIA

2008-07-23T00:29:00.026+08:00

Mechanical Design > Wireframe and Surface Design

Select Start > Mechanical Design > Wireframe and Surface Design. Then you'll be asked for a new part name. Enter a name as you like and check on enable hybrid design. Press OK.

In the workbench, click on the arrow just below the Spline icon, a toolbar will come out and then click on the Helix icon. Alt: Insert > Wireframe > Helix. A Helix Curve Definition box will appear as shown below.

Right click in the Starting Point box and select Create Point. In the Point Definition box that appeared, let the Point Type as Coordinate and enter 30mm for the X-coordinate and let the rest as default. Press OK. Then, right click in the Axis box and select Z Axis. You should now obtain a helix as shown. Just press the Preview button but not the OK button.

Now edit the Pitch to 10mm and the Height to 100mm. Let other values by default and press OK.
Now you'll get a helix as shown below.

To create the profile of the spring, we would have to switch into the Part Design Workbench. Start > Mechanical Design > Part Design. Select the zx-plane and click on the Sketch icon. Create a Circle of Diameter 5mm just on the end point of the Helix as shown below.

Exit the Sketcher Workbench to return to the Part Design Workbench. Click on the Rib icon and in the Rib Definition box, select Sketch.2 (circle) as the Profile and the Helix as the Center Curve. Press OK button to obtain your spring.