Leonard Sampson is a machine tool designer, and has more than 15 years of Catia experience. He also has over 23 years of Autocad experience
Just for peace of mind, I would like readers to understand my qualifications. I was formally trained by InCat about 10 years ago, and at this time have approximately 15 years of experience with Catia V5. I am a machine tool designer, and have extensive understanding of CatPart, Catproduct, and finite element analysis. I have some basic knowledge of wire frame as well. Generally, I am comfortable with the software, and would love to hear feedback for future tutorials.
Overview of Catia V5 Tutorial 2: Using CatPart commands
Today we are covering two of the basic commands you will use when you are beginning Catia. We covered the sketch command in the first tutorial, and I would refer you there if you have any questions in regards to the 2D sketching capabilities of Catia. For this Hub, we will be specifically covering the pad command, and the pocket command.
The pad command is the primary command to ad volume to a solid in Catia V5. It generates a sketch based extrusion. The pocket command is the counterpart to the pad command. Pocket is used to remove volume from a 3D solid, it is also generates a negative extrusion based on a sketch.
With these two commands, along with sketch, you will be on your way to understanding the basics of Catia V5 design. While there is a long way to go, these are by far the most commonly used commands in Catia, in its basic licensing forms.
The Pad Command
The Pad command is the first command on the standard toolbar in the Catpart shell. It appears as two cubes, with one proud of the other. If you look at this button on the toolbar, you may notice that it has a small down arrow on it. This is for sub-commands within the pad command family. Included is Drafted Pad and Multi-pad. We are not going to cover those in this tutorial, but I may consider it if it seems that people are interested.
You can select the pad command before you have drawn any sketch. It will not work.
Once you have created your sketch on the plane you wanted the sketch to be on, you can "pad" the sketch. To pad the sketch, you will either select the sketch, in the 3d space, or on the tree, then you select the pad command. You can also select the pad command first, and it will prompt you to select a sketch to pad. It will default direction to perpendicular of the plane the sketch was drawn on. It will also default to a specific length. When I pad on my version of Catia, it defaults to a 20mm thick extrusion. From this point there are several things you can do with the command. Let's cover them as they appear in the dialog box.
The top of the dialog box consists of a pull down menu called "Type:" a "Length:" section that accepts text and a "Limit:" area that is grayed out as the default.
The Type is defaulted to dimension and this will be your primary mode of creating a pad. It basically means you will be manual entering a number for your pad thickness, that number is entered in the "Length:" box, right below the "Type:". But there are other options which will come in handy as well...
Dimension: Manually enter the data for a pad thickness
Up to Next: (This command is very very picky!)This will extend the pad up to the next solid within that specific PartBody. If that limit changes, the pad will automatically change as well. Also, the dialog box changes when you select Up to Next. The Length box is removed, and replaced with two different boxes. a Limit box, which is used to select a item to Pad up to Next. There is also a Offset box. This is a number you can offset the start of the extrusion from the sketch surface. Meaning you do not have to start the solid at the surface of the sketch, you have control over that start point as well.
Up to Last: (This command is very very picky!)This command will effectively extrude your pad to the furthest surface within the specific PartBody. If that limit changes, the pad will automatically change as well. Also, the dialog box changes when you select Up to Last. The Length box is removed, and replaced with two different boxes. a Limit box, which is used to select a item to Pad up to Last. There is also a Offset box. This is a number you can offset the start of the extrusion from the sketch surface.
Up to Plane: Very useful if you like to work with planes. You can set a plane and extrude your pad to that specific plane. If the plane changes so does the pad. Also, the dialog box changes when you select Up to Plane. The Length box is removed, and replaced with two different boxes. a Limit box, which is used to select a item to Pad up to Plane. There is also a Offset box. This is a number you can offset the start of the extrusion from the sketch surface.
Up to Surface: This allows you to pick a surface you would like to extend your pad to. It must be within the existing PartBody to work. Otherwise you can use Up to Plane. Also, the dialog box changes when you select Up to Surface. The Length box is removed, and replaced with two different boxes. a Limit box, which is used to select a item to Pad up to Surface. There is also a Offset box. This is a number you can offset the start of the extrusion from the sketch surface.
Those are the primary commands for Pad, but there is more...
Under the 'First Limit' Box, there is a second box called 'Profile/Sketch'. In this box there are a few items to cover. The 'Selection' window is the area you will want to highlight when selecting a sketch to extrude. If the sketch is highlighted before you select the pad command, you will not need to do anything. If it is not, you will want to make sure the area is highlighted, then with your cursor, select the sketch to pad.
Below the 'Selection' window:
'Thick' check box: Clicking the checkbox will expand the dialog box, in the new area, the lower right hand section is the area you can set your "thickness" This thickness is wall thickness, if you want your solid to be hollowed through, like tubing.
Reverse Side Button: The 'Reverse Side' button is also in this section. The reverse side command can change whether the solid will be within the sketch or outside of the sketch. It only works with more complex sketches, with inner and outer boundaries.
Below the 'Profile/Surface' window:
Below the there are a few commands to look at. There is also 'OK', 'Cancel', and 'Preview', which I believe to be fairly self explanatory.
'Mirrored extent' check box: This will mirror your extrusion to both sides of the sketch, this is defaulted off, and your sketch will extrude in one direction only, unless checked.
'Reverse Direction' button: Another fairly straight forward command, hitting this button will extrude the sketch in the opposite direction.
'More' button: The more button will extend the dialog box, for some additional commands.
The 'More' button commands:
The More button commands are some commands that will be extremely useful as you become more proficient with Catia V5. They take what is a basic command and give you some additional controls to minimize tree structure clutter and simplify the overall complexity of your modeling.
Second Limit: The second limit area will give you the same option you have in first limit. The purpose of second limit is to give you control over your sketch in multiple directions. It is similar to Mirror extent, but it has the bonus of allowing you to not just mirror, but make each direction unique. This includes negative values, which means you can start your solid at some distance other than where your sketch surface is.
Direction: This area can be a little tricky. This area gives you the ability to modify the direction of the solid if you need it to be different than perpendicular to the sketch. You will see the 'Normal to profile' box is checked, meaning it will extrude perpendicular to sketch, this is default, but if you highlight the 'Reference' section, you can choose planes, or lines or many other objects to change to direction.
So, that is all the commands and options with Pad. We will move onto Pocket. I suspect it will be less wordy, since a lot of the commands are exactly the same as pad.
The Pocket Command
The pocket command is a lot like pad, but instead of adding volume to a solid, we will be removing volume from a solid with pocket. When you select the 'Pocket' command you are prompted with a dialog box that looks to be identical to the 'Pad' Command. It is, and the commands work in the same way. I will recap quickly and for more detail you can look up at the Pad section to see more information.
First limit appears at the top of the dialog box. This area includes 'Type', 'Limit", and 'Offset' These commands determine the length of your extrusion, or in this case, depth of your pocketing.
Profile/Surface is the section just below first limit. This is the area that you select your profile, and Thick toggle as well. The thick toggle works in the inverse as the thick for pad. So instead of giving your pad a hollowed center, it will leave the center material, and only remove your set wall thickness.
Mirrored extend is your next toggle button, and below that is your Reverse Direction button. These both work exactly as the pad version functions.
Below that is the More button.
The More commands are also the same as Pad. At the top you have the Second Limit area, which works identical to the Pad Command. Below that you have the Direction area, which also works exactly the same as Pad.
That's it! Pad and Pocket Commands explained for Catia V5. I hope this helps you understand some of the ability these commands have to offer, beyond simple solids.
© 2018 Leonard L Sampson