Wednesday, June 27, 2012

Catia v5 Tutorial: Multi-section Solid and Shell

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.

Tuesday, June 26, 2012

Catia v5 Tutorial: Rib and Slot

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.




Monday, June 25, 2012

Catia v5 Tutorial: Shaft and Hole

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.