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3D Solid Body Operations
Performing 3D Solid Body Operations
Keep in mind the data entry and graphic cursor construction techniques described in the Geometry Overview. The same rules for performing 3D solid body operations, including booleans, imprints, clippings, thickens, blends, copies, Body-Solids, etc., will also apply. The mouse cursor is used for locating control points in the Model View, and the input fields in the Geometry tab in the Input dialog override the cursor location.
The following describes the use of 3D solid body operations for constructing complex solid bodies in StressCheck.
Target & Tool Bodies
For example, a boolean operation requires as input two or more bodies, one of which is designated as the target body (highlighting green with selection), and the remaining bodies are designated as tool bodies (highlighting red with selection).
The target body is generally the object which survives after the boolean operation is performed, and is typically a solid body for 3D solid body operations. The tool body (or bodies) may be solid or sheet, depending on the type of boolean operation. When performing a boolean operation, you are designating existing solid bodies (and potentially sheet bodies) as input to a boolean operator, and the result is one or more solid bodies. The definitions of each target body, tool body (or bodies) and boolean operator are preserved in StressCheck’s data structure.
The result body (or bodies) may then be used as input to a subsequent boolean, blend, clipping, copy or other 3D solid body operation. Although a tool body may be suppressed from the Model View, its definition remains in the StressCheck data structure, and its dimensions may be modified either through an edit operation or through a parametric change.
For an example of 3D solid body operations, refer to StressCheck Tutorial: Solid Modeling of Threaded Holes.
Preparing for 3D Solid Body Operations
Before creating a new solid body via a 3D solid body operation, you must first set the Reference/Theory/Units Toolbar to 3D and select Class > Geometry or the Geometry tab in the Input dialog. As described in the Geometry Overview, 3D solid body operations also rely heavily on the Class > Action > Object > Method (C/A/O/M) command paradigm. In 3D solid body operations the most important Action is of course Create.
To access geometric construction of 3D solid body objects, first enable Surface in the Surface/Curve Selector:
Note: by default solids are a dark blue color (Figure 1b), whereas surfaces are a bright blue color (Figure 1c).
Once a 3D solid body object/operation has been selected a method must be chosen. While not all methods may be appropriate for every 3D solid body object/operation, each method works in a consistent way for every corresponding 3D solid body object/operation. Brief descriptions of each 3D solid body creation method are included below.
Boolean (Body) Operations
To access the boolean operations for 3D solid bodies, change the C/A/O/M to Create > Body, then select one of the below methods.
Bool-Union Method
The Bool-Union (boolean union) method is used to create a new solid body by performing a union between two or more intersecting solid bodies, or one solid body and one or more intersecting sheet bodies. There can only be one target (several tool objects are possible) object for a boolean union operation. Simply select the target solid body (which will highlight green), then the tool solid/sheet body (or bodies, which will highlight red), and click Accept or hit the Enter key.
Note: when unioning combinations of solid bodies and sheet bodies, solid bodies should be unioned first, followed by the union of the resulting solid body (or bodies) with the sheet body (or bodies).
Figure 2a shows two solid bodies (box and cylinder) and one sheet body (circle surface) before a boolean union operation, and Figure 2b shows the result of first unioning the box and cylinder to create a new solid body, and then unioning the resulting solid body with the circular surface.
Note: for the union of the two solids, only the external surfaces are preserved, while the internal surfaces are trimmed (because the tool is a solid). Conversely for the union of the surface and solid, where the tool is a surface, only the internal surfaces are preserved while the external surfaces are trimmed. It may be very useful to embed a surface into a solid, for example to represent a crack surface (or surfaces) for a 3D fracture mechanics analysis. In this case, the solid body would be the target, and the tool body would be the crack surface (or surfaces). The result would be a solid body with the designation of general body, since it now contains internal surfaces.
The Bool-Union-Gen (boolean union general) method may also be used to union targets and tools, but more flexibility is available regarding the trimming performed on the result body.
Bool-Union-Gen Method
The Bool-Union-Gen (boolean union general) method is used to create a new solid body by performing a union between two or more intersecting solid bodies, or one solid body and one or more intersecting sheet bodies, with the option to trim internal, external or no geometric boundaries (i.e. curves and surfaces). There can only be one target (several tool objects are possible) object for a boolean union general operation. Simply select the target solid body (which will highlight green), then the tool solid/sheet body (or bodies, which will highlight red), select a Trim: option, and click Accept or hit the Enter key.
Note: both Bool-Union and Bool-Union-Gen methods use the same Parasolid function. The difference is that the Bool-Union-Gen method gives the user control over what surfaces are retained (Trim:) after the Boolean operation, especially when unioning sheet and solid bodies. The Bool-Union method always retains sheet body, but not solid body, surfaces internal to the unioned body. This is convenient for embedded crack faces, for example.
Trim Options
- None: Default. No trim is performed (all curves and surfaces will remain).
- InSolid: Trim is performed inside resulting body (in solid) to remove interior curves and surfaces.
- InVoid: Trim is performed outside resulting body (in void) to remove exterior curves and surfaces.
When using the Bool-Union-Gen method to union a solid and a sheet body, you can get the same result as the Bool-Union method by selecting trim in void (“InVoid”, meaning outside the body). Alternately if you Boolean union a solid and a sheet and use trim in solid (“InSolid”, meaning inside the body), then it will remove the interior (embedded) surfaces and leave the surfaces outside the body. If you use “None”, which is the default, you will retain the surfaces inside and outside the solid body, but get a single general body as a result.
Figure 3a shows three solid bodies (box, cylinder and torus) before a boolean union general operation, and Figure 3b shows the result with Trim: None and geometric transparency on.
The Bool-Union-Gen method is very useful for generating one solid body containing multiple different regions which are bonded, embedded or fused. In this way, a continuous automesh may be generated across the regions but different material assignments may be made to each region via Mesh Region.
Bool-Subtract Method
The Bool-Subtract (boolean subtraction) method is used to create a new solid body by performing a subtraction between two or more intersecting solid bodies. There can only be one target (several tool objects are possible) object for a boolean subtraction operation. Simply select the target solid body (which will highlight green), then the tool solid body (or bodies, which will highlight red), and click Accept or hit the Enter key. Note: the target solid body is the solid body expected to remain after the boolean subtraction operation.
Figure 4a shows three solid bodies before a boolean subtraction operation, and Figure 4b shows the resulting solid body. In this case, the box was the target body.
Bool-Intersect Method
The Bool-Intersect (boolean intersection) method is used to create a new solid body by computing the shared region(s) between two or more intersecting solid bodies. There can only be one target (several tool objects are possible) object for a boolean intersection operation. Simply select the target body (which will highlight green), then the tool body (or bodies, which will highlight red), and click Accept or hit the Enter key.
Figure 5a shows three solid bodies before a boolean intersection operation, and Figure 5b shows the result.
Stitch Method
The Stitch method makes it possible to construct a single solid body by sewing multiple surface patches together. Simply select a group of sheet bodies which will represent an enclosed volume and click Accept or hit the Enter key. The resulting body will automatically become a solid body if possible. You may adjust the Parasolid enclosure tolerance (Tol:) if necessary.
For example, we can construct a solid cylinder by sewing circular surfaces at the ends of a cylindrical surface (Figure 6a). The resulting solid cylinder body is show in Figure 6b.
Clipping Operations
The purpose of a clipping operation is to divide a body into two sections, and then subtract the portion of the solid object which lies on one side or the other of the clipping surface. The direction of the normal vector for the clipping surface determines whether to use a Clip-Back or a Clip-Front operation. You can see the vector triad by placing the cursor on the clipping surface. Left click on the solid body (green highlight), then the clipping surface to perform the clipping operation (no Accept is necessary).
Figure 7a shows the solid body and sheet body (plane) before a clipping operation.
Note: The clipping surface may be any type of surface, not necessarily a plane. Also, If your model is parametric, make sure that the clipping surface is also parametric so that it will encompass the entire object to be clipped, regardless of the dimensions corresponding to any given set of parameter values.
To access the clipping operations for 3D solid bodies, change the C/A/O/M to Create > Body, then select one of the below methods.
Clip-Back Method
The Clip-Back operation will remove the solid geometry on the back (negative) side of the clipping surface. Figure 7b shows the result of a Clip-Back operation on the geometry of Figure 7a.
Clip-Front Method
the Clip-Front operation will remove the target body that lies on the positive side of the clipping surface. Figure 7c shows the result of a Clip-Front operation on the geometry of Figure 7a.
Body-Imprint Operations
Body-Imprint methods are provided to make it possible to create new edges and faces in an existing target body, usually for the purpose of performing subsequent solid body construction operations using the new faces. The methods provided are: Both Bodies, Target Body, Curve Normal, Curve Vector, Faces, and Plane.
Note: for the Curve Normal, Curve Vector and Plane methods, the default tolerance 10-5 is used. If the imprint operation fails or does not perform as expected for this default tolerance, try a smaller value in the Tol: field.
To access the imprint operations for 3D solid bodies, change the C/A/O/M to Create > Body-Imprint then select one of the below methods.
Both Bodies Method
Select a target body (green highlight) and a tool body, and the imprint will automatically be performed. The curve(s) representing the intersection(s) between the selected tool body and the target body will be imprinted on both the target body and the tool body.
Figure 8a shows two solids before a Both Bodies operation, and Figure 8b shows the resulting bodies. Note the new boundaries in each body where the two bodies intersect.
Target Body Method
Select a target body (green highlight) and a tool body, and the imprint will automatically be performed. The curve(s) representing the intersection(s) between the selected tool body and the target body will be imprinted only on the target body.
Figure 9a shows two solids before a Target Body operation, and Figure 9b shows the resulting bodies when the target body is the box. Note the new boundaries only appear on the box where the torus intersected it.
Curve Normal Method
Select a target solid body (green highlight) and then select one or more curves (red highlight), and click Accept or hit the Enter key. This will imprint the selected curve(s) on the selected solid body by projecting them locally down face normal. You must click on the Accept button to initiate the operation after picking the final curve.
Figure 10a shows a solid body and two spline curves to be imprinted, and Figure 10b shows the result.
Note: in some cases it may be necessary to update the imprint tolerance (Tol:) to ensure the result is as expected. Also, care must be taken to ensure that the selected curves are not associated with a body which will undergo future 3D solid modeling operations.
Curve Vector Method
Select a target solid body (green highlight) and then select one or more curves (red highlight), optionally hold Ctrl + Shift and select a local system, then click Accept or hit the Enter key. This will imprint the selected curve(s) on the selected sheet body by projecting them in the specified system’s Z axis direction.
- If no local system is supplied, the direction of projection corresponds to the direction of the positive global Z axis.
- If a local system is selected , the direction of projection corresponds to the direction of the positive local Z axis.
Figure 11a shows a solid body and two spline curves to be imprinted using the local Z axis shown, and Figure 11b shows the result.
Selection of a local system Z-axis is most applicable working with sheet or solid bodies in 3D space. When working with sheet bodies in 2D (Planar) space, the Curve Normal method and Curve Vector method with no local system selected will be identical.
Note: in some cases it may be necessary to update the imprint tolerance (Tol:) to ensure the result is as expected.
Faces Method
Select a target body (green highlight) and one or more faces of neighboring bodies, and then click Accept or hit the Enter key. The curve(s) representing the intersection(s) between the selected faces and the faces of the target body will be imprinted on the target body. You must click on the Accept button to initiate the operation after picking the final face.
Plane Method
Select a target body (green highlight) and one planar sheet body, and the imprint will automatically be performed. The curve(s) representing the intersection(s) between the extended plane of the surface and the faces of the target body will be imprinted on the target body. The sheet body will be suppressed from view.
Body-Trim Operations
Body-Trim operations work by removing a selected trimmed surface (or surfaces) from a solid body. To access the trim operations for solid bodies, change the C/A/O/M to Create > Body-Trim > No Heal. Next, select one or more surfaces within the solid body (red highlight). Then, click Accept or hit the Enter key to trim the surfaces from the solid body.
Note: care must be taken to ensure that the result of the trim operation is a valid solid, especially if planning to automesh the result.
Body-Copy Operations
Body-Copy operations a way to copy an existing body and to orient the copy anywhere in space. To access the copy operations for solid bodies, change the C/A/O/M to Create > Body-Copy then select one of the below methods.
To perform the copy, select the body and a reference system (they will both highlight red). The reference system is needed in order to identify a reference location in the body and the orientation of the parent body. Then, you may supply the location and orientation of the copy using the input fields. Alternatively, if you hold Ctrl + Shift and select an existing local system (other than the previously selected reference system, it will highlight green) the copy will be attached to the second system and the input field values will be relative to the second local system. Finally, click Accept or hit the Enter key to create the copy.
Figure 12a shows a solid body, reference system and second system, and Figure 12b shows the resulting copy with all input fields = 0.
Child Method
The Child method will construct a copy of the selected solid body and retain a connection to the original so that if the parent solid body is parametric and dimensions are changed, the copy will automatically be updated, and thus remain a consistent copy of the parent.
Orphan Method
The Orphan method will break the connection to the parent solid body so that if the parent dimensions are changed, the copy will not inherit the change. Additionally, this allows the parent solid body to be deleted.
Body-Solid Operations
Body-Solid operations allow sheet bodies to be converted to 3D solid bodies. The following Body-Solid methods are provided: Extrude, Extrude Face, Spin, Spin Face, Sweep, and Thicken. To access Body-Solid operations, change the C/A/O/M to Create > Body-Solid then select one of the below methods.
Extrude Method
Select a sheet (surface) body that will be extruded to form a solid body, by specifying distances or selecting objects as limits for the extrusion. The limit inputs are determined by the options in the Limit1 and Limit2 combo-boxes. Select a local coordinate system (while holding the Ctrl + Shift keys, it will highlight green) to determine the direction of the extrusion (along the positive Z-axis). If no system is selected, the extrusion will be relative to the positive global Z-axis. The local system should be selected before selecting the profile surface (red highlight) or limiting objects. The extruded solid body will be created automatically after the final required object is selected.
There are several methods for extruding a surface to form a solid, which relate to the location of the front and back faces of the extruded solid. The methods for defining the front and back faces may be used in any combination. The Distance method requires as input the distance from the profile surface where the front and back faces should be located. The other methods (Face and Surface) require as input the number of limiting faces which occur between the profile surface and the limiting surface of the extrusion. If the limiting faces are located in a negative direction relative to the local system Z axis (or global system Z axis if no local system is selected), the input limit should be provided as a negative value.
Note: the order of selection of faces should be consistent with the Z-axis of the local coordinate system. To define the limit values for Face and Surface, you can choose any positive integer number for the face facing the positive Z-axis of the plane, and any negative integer number for the face facing the negative Z-axis of the plane. The options for specifying the limits of an extruded solid are described below.
- Distance – specify the distance from the selected surface to the front/back face of the solid. “Dist1” refers to the front face, “Dist2” refers to the back face. Negative distance is measured relative to the positive normal of the surface.
- Surface – Select a surface that will be used as the front or back bounding face of the extruded solid.
- Face – Select the face of a body that will be used as the front or back bounding face of the extruded solid.
The below animated example demonstrates the use of the Extrude method with Limit1: Distance and Limit2: Face. Set Dist1: 0, Limit2: 1, hold Ctrl + Shift and select the ellipse system, then select the ellipse, then select the back face of the box in the positive Z. The ellipse surface will be extruded from its current location to the back face of the box.
Now, set Limit1: Face and Limit2: Distance. Set Limit1: -1, Dist2: 0, hold Ctrl + Shift and select the ellipse system, then select the ellipse, then select the back face of the box in the negative Z. The ellipse surface will be extruded from the back face of the box to its current location.
Extrude Face Method
Select the face(s) of a solid body that you wish to extrude (red highlight), provide the length of extrusion (Dist:), and click Accept or hit the Enter key. By default, the extrusion is performed in the direction of the positive Z-axis of the global system. To select a local system, hold the Ctrl + Shift keys while picking a local system object in the Model View.
A typical usage of this function is to imprint a curve onto an existing face of a solid body, then extrude into the body to form a slot, or away from the body to form a tab. Supply as input the length of the extrusion, then click the solid face(s), then click Accept or hit the Enter key to perform the extrude operation. This is demonstrated in the below animated example with Dist:5.
Spin Method
Specify a sheet (surface) body to be spun about the Z-axis of a local system to form a solid. The local system must be selected while holding the Ctrl + Shift keys (green highlight). The local system must be selected before selecting the surface. If no local system is supplied, the spin will be performed about the global Z axis. Supply the Angle (in degrees) that the surface will be spun about the Z axis. Then, select the sheet body (red highlight) and click Accept or hit the Enter key to create the spun solid body.
A typical usage of this function is to create a 3D sector of an axisymmetric solid. This is demonstrated in the below animated example with Angle:45.
Spin Face Method
Specify the face(s) of a solid body that you wish to spin about the Z-axis of a local system. The local system must be selected while holding the Ctrl + Shift keys (green highlight). The local system must be selected before selecting the face(s). If no local system is supplied, the spin will be performed about the global Z axis. Supply as input the Angle (in degrees) to spin the face(s) about the corresponding Z-axis. Then, select the face(s) of the solid body (red highlight), and click Accept or hit the Enter key to create the spun solid.
A typical usage of this function is to generate a curved extrusion from a set of solid faces. This is demonstrated in the below animated example with Angle:45.
Sweep Method
Construct a solid body by sweeping a profile sheet body (surface) along a path curve, with the cross section at any location along the path curve maintaining its original orientation relative to the path curve. First select the profile surface (red highlight), then the path curve. The swept solid body will be created automatically after the path curve selection.
A typical usage of this function is to sweep a cross section into a solid. This is demonstrated in the below animated example.
Thicken Method
The Thicken method will convert a sheet body (a surface with no thickness) into a solid body with the supplied thickness values. The existing surface will be treated as a mid-surface, to which material will be added in the positive and/or negative directions with respect to the normal at each point on the surface. Supply the distance(s) in the positive (Above: input field) and/or negative (Below: input field) direction(s) to extend the volume of the solid body, and then select a sheet body or general body that will be thickened. The thickened solid body will be created automatically after the sheet body selection.
A typical usage of this function is to extrude a cross section normal into a solid. This is demonstrated in the below animated example for Above: 0.5 and Below: 0.3.
Note: when the sheet body is planar, the Thicken method and Extrude method will produce the same result.
Blend Edge Operations
Blend Edge operations may be used to create rolling ball or variable radius blends, fillets and chamfers in a solid body. For detailed stress analysis, it is important to model regions of interest with smoothly connected boundaries. Note that the edges to be selected for application of the edge blend must all belong to a single solid body.
To access the Blend Edge operations for solid bodies, change the C/A/O/M to Create > Blend Edge then select one of the below methods.
Rolling Ball Method
Computes a rolling ball fillet radius based on the selection of one or more curves (red highlight) belonging to the same solid. Supply a rolling ball radius in the Radius: input field, select the curve(s) and click Accept or hit the Enter key.
A typical usage of this function is to blend two or more discontinuous surfaces into a smoothly connected boundaries. This is demonstrated in the below animated example for Radius: 0.25.
Variable (Var.) Radius
A variable radius blend is characterized by 6 parameters: two radii at each end (R1-a, R1-b, R2-a, R2-b) and a shape factor at each end of the blend (Rho1, Rho2). The following situations are possible depending on the selection of these parameters:
- If all radii are equal and Rho1=Rho2=0, then the blend has a circular cross section.
- If different radius values are specified on each side and the Rho values are zero, then the blend has an elliptical cross section.
Further control of the shape of the cross section is obtained by setting Rho to non-zero values:
- Rho between 0.0 and 0.5 for elliptical cross section.
- Rho= 0.5 for a parabolic cross section.
- Rho between 0.5 and 1.0 for hyperbolic cross section. As Rho approaches 1.0, the blend becomes more and more L-shaped. Rho should be always strictly less than 1.0.
Supply the radii and Rho values at each end, select the curve(s) and click Accept or hit the Enter key. This is demonstrated in the below animated example for R1-a: 0.2, R1-b: 0.4, R2-a: 0.8, R2-b: 1.6, Rho1: 0 and Rho2: 0.
Chamfer Method
A chamfer is a flat blend which replaces the selected edge(s) with a flat face, where the distance from the original edge on the selected face is distance “R1”, and the distance from the original edge on the neighboring face is distance “R2”. To specify the face corresponding to where the distance “R1” will be measured, hold the Shift + Ctrl keys and select the surface. Click Accept or hit the Enter key to perform the chamfer.
The Chamfer method is useful for generating countersink holes, transitions and stepped geometry. This is demonstrated in the below animated example for a countersink hole with R1: 0.1 and R2: 0.2.
Blend Face Operations
To access the Blend Face operations for solid bodies, change the C/A/O/M to Create > Blend Face > Rolling Ball.
A rolling ball face blend operation is essentially a hybrid between the surface fillet and the edge blend operations. In the case of the face blend, you must distinguish the “right” wall of the blend from the “left” wall of the blend. You may pick right and left wall faces in any order, as long as you hold the Ctrl + Shift keys to distinguish them while picking. For example, select the left wall faces (red highlight), then hold the Ctrl + Shift keys and select the right wall faces (green highlight). Then click Accept or hit the Enter key to perform the blend face operation.
For the face blend, there are two cases which are valid:
- All left and right wall faces belong to the same body.
- All left wall faces must belong to one general body and all right wall faces must belong to a different general body.
The Blend Face method is useful for generating transitions between intersecting surfaces. This is demonstrated in the below animated example for Radius: 0.5.
