CATIA V5 Bottle Designing TRY IT!!!

Unique Shaped Bottle in CATIA V5

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.

POSTED BY RIDHUAN AT 04:32 14 COMMENTS  LINKS TO THIS POST

 GENERATIVE SHAPE WORKBENCH PART DESIGN WORKBENCH

THURSDAY, DECEMBER 9, 2010

Modeling Fan or Propeller Blades

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.

Modeling Universal Joint in CATIA V5

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.

Make a Guitar with CATIA

Mechanical Design > Assembly Design

Start the Assembly Design Workbench by selecting Start > Mechanical Design > Assembly Design or File > New > Product. Rename the product toGuitar (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 Linetool 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 (pressctrl 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 theGuitar 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 PartBodysection.



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 theSketch 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 materialto make the guitar more beautiful. The guitar is now complete. Later actions are up to u.

POSTED BY RIDHUAN AT 02:54 2 COMMENTS  LINKS TO THIS POST

  

SATURDAY, OCTOBER 25, 2008

Making An Assembly

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 > Productwhich 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. (theUndo 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 theManipulation 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.

Modelling a Spring in CATIA

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 thePoint Definition box that appeared, let the Point Type asCoordinate 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 Previewbutton 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 thePart Design Workbench. Start > Mechanical Design > Part Design. Select the zx-plane and click on the Sketch icon. Create aCircle 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 Definitionbox, select Sketch.2 (circle) as the Profile and the Helix as theCenter Curve. Press OK button to obtain your spring.

Welding Design in CATIA

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.

Making a Pad, Pocket, Fillet and Chamfer in Part Design Workbench

Mechanical Design > Part Design

Open the xxx.CATPart file used in Basic Sketching in Sketcher Workbench. If you are still in the Sketcher Workbench, click on the Exit workbench icon to go to the Part Design Workbench.

 
Making a Pad. Select Sketch.1 from the Design Tree and click on the Pad icon  or select Insert > Sketch-Based Features > Pad. A Pocket Definition box will pop up and enter your desired pad length and press OK. The drawing should look like this:

 

Now we are creating a pocket on a face. Select the top face as shown below and click on the Sketch  icon.

  

You shall then be in the Sketcher Workbench. Create a circle as shown ad click the Exit Workbench icon. While the sketch is selected, click on the Pocket icon  Alt: Insert > Sketch-Based Features > Pocket. A Pocket Definition box will appear and enter the desired length of the pocket. Press Preview to preview or just press OK.

 

Making a Fillet. Switch the Shading mode  to Shading with Edges. Click on the Edge Fillet  icon on the Dress-Up Features toolbar or select Insert > Dress-Up Features > Edge Fillet. Edge Fillet Definition box will appear and select the edge as shown for the Object(s) to Fillet. Preview the fillet and press OK.



  

Making a Chamfer. Click on the Chamfer icon  on the Dress-Up Features toolbar. Alt: Insert > Dress-Up Features > Chamfer. In the Chamfer Definition box, make sure the Mode is Length1/Angle. Change the Length 1 value to 5mm and select the edge Pocket.1 for the Object(s) to chamfer as shown in the figure. Preview and press OK.

 

Modelling the RSS Feed Icon

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.

Modeling a Simple Heat Exchanger

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..

Modeling a Simple Heat Exchanger - Continued

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.

Bolt & Nut - Threading

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 theConstraint 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.

Basic Sketching using Sketcher Workbench

Mechanical Design > Sketcher 

Select Start > Mechanical Design > Sketcher from the menu bar. Alternative: Select File > New and select Part from the list.

 or 

Enter Part name and click OK. You'll enter the Part Design Workbench.

Select a reference plane in the geometry area.
 or  
Click on the Sketch icon  or select Insert > Sketcher > Sketch. 

You will then enter the Sketcher Workbench.
Then click on the Rectangle icon  (or any profile as you please). Alternative: Insert > Profile > Predefined Profile > Rectangle. Click on any spot for a starting point and move the cursor to any position.
The dimension of the rectangle will be affected by the grid when the Snap to Point  is activated.
Adjust the dimensions by using the Constraint command. Click on the Constraint icon  and select the line profile you want to adjust (Alt: Insert > Constraint > Constraint Creation > Constraint). A dimension profile will come out and double-click on the dimension profile and a Constraint Definition box will appear where you can adjust the value.

 
Create a circle in the rectangle. Click the Circle icon  or select Insert > Profile > Circle > Circle. Click on any spot for the center of the circle and move the cursor to obtain a desired size. Resize the circle using the Constraint command.

You should have something like this:



Creating a corner. Click on the Corner  icon or select Insert > Operation > Corner. Select the horizontal and vertical lines on a corner and a curve will automatically appear. Click once again to create the corner. Some prompt may appear and click "Yes" on all of them. Once the corner is created, modify the dimension by double-clicking on the dimension constraint.

Note: If the drawing changed unexpectedly, try to fix some lines (right click on a line and select Line.X object > Fix.

 

Create a Chamfer  using the similar method of creating the Corner. You should obtain something like shown below.



Now create a hexagon using the Hexagon  icon (click on the arrow below the Rectangle icon to pop up the Hexagon icon (Alt: Insert > Profile > Predefined Profile > Hexagon).

Click on the vertical line as shown and drag the cursor to obtain the hexagon.

 

Resize the hexagon using the Constraint command and resize the circle around the hexagon.



Now we are going to trim the hexagon. Delete all the circles and constraint around the hexagon. Click the arrow below the Trim  icon on the Operation toolbar or select . Drag the pop up toolbar to other place. You should now obtain the Relimitations toolbar.

 

Now click on the Quick Trim  icon and then click on all the line you want to remove. (Alt: Insert > Operation > Relimitations > Quick Trim).

 

Now you have completed the drawing. Save the file and keep it for later use. You can click the Exit workbench  icon to go to the Part Design workbench.

Modelling a Bottle in CATIA

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.