Feature-oriented Design of Sheet Metal Workpieces

Commercial CAD systems are not properly suited for complex components
Unquestionably, the CAD technology provides a variety of advantages as far as construction is concerned. In the field of mechanical engineering the use of 2D CAD systems has meanwhile established as a standard. Currently on the march are 3D CAD systems, which offer even more possibilities, such as, for example, reality display or easy assembly of assembly groups.

The production data required by CAM systems can be directly made available, as a by-product, so to speak. Most of the CAD systems, however, do not meet the requirements and are consequently not properly suited for effective construction of sheet metal workpieces, as they lack functionality. This implies, for example, free-cuts of flanges, calculation of the neutral line as well as calculation of the unfolded blank. The lack of functionality can only be compensated by a higher expenditure or by (expensive) adjustments. Consequently, there is an increasing need of software packages that are tailored to the needs of sheet metal construction. With the help of these systems the time needed for design and production can be considerably reduced.

2. What is meant by "feature-oriented" sheet metal construction?
The term "feature" is another expression for "characteristic". In connection with 3D CAD technology, the term has meanwhile gained an individual meaning among experts.

During construction of sheet metal workpieces a variety of production-specific frame conditions have to be considered. As already mentioned above, the most CAD systems do not provide any support for production-related problems. Therefore, it is mainly due to application engineers, to provide the relevant features. Typical features, would be, for example:

Constant sheet thickness
Mostly constant inner bending radius
Free-cut of inserted flanges
Several flange shapes, e.g. angles or Z-Bendings
Outer and inner flanges or added flanges
Punch holes, stampings, cutouts

3. Production-oriented design of sheet metal workpieces
3.1 Definition of design parameters
The first step is to define the following parameters: Sheet thickness, standard inner radius as well as width and depth of the free-cut of inserted flanges. These preset values will be used with every new object, even if they can be temporarily adjusted for a preceding object. For the following example the values below are recommended to be used:

Sheet thickness:3 mm
Bending radius:2 mm
Free-cut:0,5 mm for depth and width

Fig. 1: Definition of design parameters

3.2 Definition of the base
Normally, designing starts by defining a base, to which the chamfered areas are added. Length and width of the base have to be entered. Sheet thickness must not be neglected, as otherwise, for example, collision controls would produce incorrect results. Sheet thickness was already defined when specifying the design parameters.

3.3 Free-cut of corners
Corners, at which bending zones will meet, should be free-cut in order to assure a smooth transition. Depth and width of the free-cut is calculated from material thickness, bending radius and a tolerance value. In our example the corner free-cut is 5,5 mm

3.4 Adding of chamfers
With the help of the so-called flange functions the bending zones and the associated area are added to the base. A variety of different flange types is available:

Non-rounded flanges
Rounded flanges
Z-Büge
Contour flanges
Profile flanges

With the help of contour or profile flanges you can add flanges of any contour to the respective base. There are three possibilities, to add the base:

3.4.1 Overall dimension flange
Here, the overall dimensions of the base will be automatically reduced in a way, that the overall dimensions of the object are equal to those of the original base. This is what is mostly occurring during designing, as the respective overall dimensions are normally present.

3.4.2 Inside dimension flange
Here, the overall dimension of the base will only be reduced by the bending radius, i.e. the new dimensions are increased by sheet thickness. The inner side of the added flange is equal to the original base.

3.4.3 Added flange
The flanges are added to the available base, i.e. the overall dimensions
are increased by bending radius and sheet thickness.

3.5 Inserted flanges
These types of flanges are only partially chamfered, i.e. the bending zone does not cover the entire base. The associated parameters have to be defined accordingly, so that the flange can be shortened at the left and right side as desired. Furthermore, the free-cut of flanges will take effect. The material adjacent to the flanges will be free-cut by the specified values, in order to prevent the sheet from being torn during bending.

3.6 Extension of flanges
The previously inserted flange must often be extended. To fulfil this task, the system must be able to find and modify flanges. In our example, the inserted flange will simply be extended up to the desired position. The position can be determined by any point or area. If the flange is extended to a specified area, you can enter a gap between the flange and the area, in order to compensate possibly occurring production tolerances.

3.7 Editing flanges
During sheet metal design, there are, of course, sufficient features, which can be created by the standard functions of a CAD system. These should be used as often as possible. A typical example would be the rounding of flanges.

3.8 Close corners
Due to the free-cut on the base the corners of adjacent flanges are not closed.
There are a variety of special functions which allow you to close these corners. Examples:

Close with flush joint
Close with overlap
Close with free-cut

With every function you can define a gap to compensate tolerances.

Often, sheet metal workpieces do not only contain standard punch holes, such as bores, rectangular holes or slots, but also different shapes required for reasons of functionality. Standard punch holes are provided with the standard sheet metal design software package, whereas for non-standard shapes the CAD system will be used. The shape is drawn with the CAD functions, parameterised and, for example, immediately added to a tool library. In this way, the available punching tools can be reloaded at any time, which considerably simplifies the design process.

4. Calculation of the unfolded blank
One of the most important features of sheet metal design is the quick and easy calculation of the cut. The data of the workpiece are extracted and transferred from the CAD system to a Solver.

In this way, for example, sheet thickness can either be modified or can directly be taken from the workpiece. For calculation of the neutral line different methods are available. In addition to DIN 6935, the contracting factors can be taken from a material data table, machine-specific allowance values can be used or the position of the neutral line can be estimated on the basis of experience.

There are two possibilities to create the cut: You can use the position of the neutral line as basis for the cut. The result would be a flat pattern. It may, however, also occur, that another part, a so-called intersection part intersects the workpiece. To obtain the intersection line, calculation of the unfolded blank has to consider both top and bottom part of the workpiece. Each side has different intersection lines. Optionally, the maximum required intersection line can be indicated, provided that the cut is < 90° as compared to the flat pattern. Intersection lines are not only resulting from calculation of the maximum cutting edge of intersecting parts but also, if for example, the punch holes are within bending zones. The intersection lines normally consist of many short straight lines, which are, however, not well-suited for CNC-controlled machines.

For this reason, the number of reference points for the intersection lines can be reduced to a minimum by defining a maximum offset from the actual intersection line, e.g.. 0,1 mm. The number of reference points can be reduced linearly or can be approximated with the help of arc segments within the range of the defined offset. The reference points can be changed to arc segments so that a tangential overlap will be the result.

The unfolded blank is calculated within a few seconds depending on how complex the sheet metal is. It includes bending lines, bending zones, all intersections, bore holes and punch holes as well as information on the punching tools used. The contour of the