Introduction to part modeling and Sketch based features

Part modeling refers to the creation of 3D models that are exact representation of the actual product that we wish to manufacture. These need to be the exact representation because based on this, the tooling is created or machine program is generated for manufacturing. The primary aim of making a sketch is to utilize it to make a 3D part. Therefore, a sketch is made keeping in mind the tools that are available in the part design workbench or other workbenches that we intend on using. The Part Design workbench comprises of variety of tools that help the designer convert the sketch into 3D model. Some designs may be difficult to model directly in the Part Design workbench. Therefore, to model those parts we take help of Wireframe and Surface design workbench, sheet metal design and other workbenches. We will see in a bit, how we use a sketch to make a part.

Following are some of the 3D parts, modeled in Catia.

Sketch based features

Sketch based features toolbar

The sketch based features toolbar is present in the part design workbench. It comprises of tools like pad, pocket, rib, slot, shaft, groove, hole, multi-sections solid etc. Each of these is a way to add / remove material in a certain way. Also, these have different requirements for sketches. Some of these are used for adding material while other are used for removing material. For example, pad, rib, shaft and multi-sections solid are used for adding material while hole, pocket, groove etc. are used for removing material.
Pad - Pad can be used to add material in a direction perpendicular to the sketch plane or in a direction that is at some angle to the sketch plane. The direction may be defined by a line that's present in another sketch. So, any of the sketch that we have made in the previous exercise can use the pad command to add material.

Pad dialogue box

You may use a sketch to add material in both the directions or in one direction. These limits can be specified using the first limit and second limits as shown. In case if the first limit is specified as 20mm and second as 55mm, and you wish to switch these, you can do so by simply selecting the Reverse direction button.

The type may be dimension i.e. you give a specified length or you may choose other options like up to next, up to last etc. The other options may work if you have already got material or surfaces present and wish to use these as limits of your pad. If you wish to extend both limits equally, you can use the option of Mirrored extent, this will remove the option of second limit.

Normally, you may add material normally to the sketch plane. However, if you wish to add material in a direction other than normal, you can select that particular line in the Reference dialogue box.

Thick option along with Thickness dimensions can be exercised if you have made an open sketch or you do not wish to make a solid body with a closed sketch. The reverse side option can be used to flip the thicknesses as you might flip the limits.  

Pad option with two limits and thick option (Circle used as sketch)

Pocket - Pocket or the other features that are used removing material, cannot be the used unless there is some material that can be removed. Pocket works on the same principle as pad, and it can be used to remove material in a direction perpendicular to the sketch plane or at some particular angle defined by a line.

Shaft - Any closed sketch can be made to revolve about the axis of the sketch or any other line. So, the material is added symmetrically about an axis. You can choose if you wish to add material only upto a certain angular limit. With thick command, you can also use open profiles. This will make a part with some thickness instead of solid. The merge ends option can be used with the open profile to merge the solid with an already existing solid. 

Shaft options (An open sketch used with thick profile option)

Groove - Groove is used to remove material by rotating a sketch about an axis, and has all other options that work exactly as they do in shaft. So, in principle it's the same as the shaft, however it is used to subtract material.

Hole - Hole command can be and should be used to make holes. While you can make it using pocket command too, it's not a good practice. You would need to select the surface on which you wish to make a hole. You would need to provide a position of the hole with the help of positioning sketch. This is basically a point that you can constrain with the help of dimensional constraints. The hole command can also be used to apply threads. A thing to keep in mind is that while threads may be applied, these are only cosmetic in nature and will be taken into account if machine program is generated.

Hole tabs for specifying depth, type and threads

Some CAD programs display threads feature when applied, Catia does not do so. However, when you apply threads the features can be noticed from the specification tree. The thread symbol is displayed around the hole. There are three tabs present. Extension tab can be used to specify whether it's a blind hole (for blind hole you can specify the depth value) or whether is upto some plane, surface etc. Beside the hole dimension, there's a button that you can use to specify tolerance values. Bottom type can also be specified using the same type as well as the direction in which the hole is being made, you can provide an alternative orientation to the hole with respect to a line if it is not normal to the surface. The Type tab can be used to specify if it's a counter bored, counter sunk or any other type of hole. The anchor point can be selected as extreme or middle. When selected as extreme, it does not form part of the the overall hole length, while in case of middle it does form part of the hole length you specify in the extension tab. Thread definition can also be applied from the thread definition tab and whether if it will be a right hand thread or left hand thread can be specified along with standard if you choose to apply it.

Rib - With the help of Pad, we added material in one direction i.e. a direction which did not change with respect to the surface on which the sketch was made. However, rib can be used to add material in a direction of a type which may not only be normal or may even change path in any direction.

To make a feature with the help of rib, a sketch as centre curve is also required in addition to the profile that you wish to use for making solid on that particular path. Profile control can be specified using Reference surface, Pulling direction and keep angle.

Rib (profile control defined by reference surface)

The keep angle may be used if you wish that the section should have the same angle with the guide curve which it maintains from the start. If you wish the section to follow the guide curve, but maintain a particular angle, this can be done using pulling direction. Reference surface option may be used to make a solid conforming to any particular surface. Guide curve and profile will be required in each case regardless of the profile control method that you use.

Slot - Slot can be used to remove material. It works in the same way as the Rib and has all controls as discussed above.

Stiffener - The stiffener option is commonly used to add strength to the parts made using castings or plastic parts made using injection molding. Stiffener can be made using two options - side and top. In case of both options, you can use an open sketch. In case of side, the line element is extruded in plane and thickness is added in direction perpendicular to sketch plane.

Stiffener created using 'From Top' option

While in case of top, multiple line elements can be used which trim among themselves to create stiffener profiles. In case of top, thickness is added in profile plane and extrusion takes place in direction perpendicular to the plane. The thickness can be added on one side or both sides of profile. To add thickness equally on both sides, neutral fiber option can be selected.

Solid combine - Solid combine is an easy way to make 3D geometries. Parts with significant variations which can more or less can be explained using just two sketches may be good candidates for this tool. However, complex objects too may be made using this, since you can always add more features and modify the object further as required. With time, you would be able to have an idea whether if it would be productive or appropriate to apply solid combine feature.

Solid combine and pocket used to make part.

In case of reverse engineering, it is specially useful if you have digital orthographic projection views that can be overlayed onto each other or if somehow we can utilize the lines of the 2D drawing directly for sketch creation. The object in this case may be easily made simply by modifying the views as sketches and combining them in the solid combine. So, reverse engineering of the part may also become relatively easy.

You can also use for use the tool for new product design too. However, it may not be as straightforward and may require some ingenuity. The part in green color, was made simply with the use of two sketches. The two sketches (red and yellow) were first combined using solid combine. Subsequently, the black color sketch was used for pocket.

Multi-sections solid - The tools (Pad, Pocket, Rib, Slot, Shaft etc.) used so far to create/remove material, utilize one section for this purpose. They may do it about a guide curve as in rib and slot or they may do it about an axis like shaft and groove. However, to create a solid that requires combination of two cross-section, we would require Multi-section solid feature.

Multi-section solid with two sections & two guides. (Guides: Blue & Light blue, Section: Green & Yellow)

Multi-section solid can be used to combine two or more sketches regardless of their cross-section type. For example, a circle may be combined with square or a square may be combined with a triangle to form a multi-section solid. In addition, we can also specify guide curves and a spine curve for the solid model creation. The closing points can be specified on each of the sketch section to get the kind of coupling we want. While you can simply connect two sections without the guide curves or even spine. In case you wish to specify guide curves there are certain conditions that you have to follow.

a) All guides should be in separate sketches. For example, there are two guide curves used in making the above solid and both are in separate sketches.
b) The guide curves should intersect the sketches. In the above feature, the light blue as well as the dark blue guide curve intersect with both the sections.

If you wish to specify spine, it should be continuous in tangency and should be kept to normal to the section planes. Not doing so will lead to unpredictable results and the solid may not be created. For creation of solid in such a manner you would also need to keep in mind the closing points that are automatically chosen (or specified) as well as the directions at these points. To enable creation, you would need to ensure that the directions are similar and points are in accordance with the solid that you wish to create. 

Remove Multi-section solid - Remove Multi-section solid works on the same principle, however it's used for removing material. So, you can specify section sketches, guide curves etc. as you do in multi-section solid and remove the material using this option.