Introduction – What’s new in SOLIDWORKS 2019

We know that we can open Assemblies in graphics only mode. This is called the Large Design Review (LDR) mode while opening assemblies. In this mode we can navigate the feature manager tree, measure distances, create cross sections, hide/show components and have walk-throughs. In SW2019 in addition to above now we can open the Assemblies while editing the assembly in LDR mode. We now have information about the MATES and Component Patterns. We can edit the supported mates but not the component patterns. This is not all. The published references can also be viewed in feature manager tree. They are not editable but connection points are visible on LMB of published references. The magnetic mates behave similar to resolved mode.

How to use the functionality?

For older version files (files not saved or created in SW2019) we need to open the files (Parts and Assemblies) in SOLIDWORKS 2019 and save them in the SOLIDWORKS 2019 version. For the newly created assemblies and parts in SOLIDWORKS 2019, this will work without saving. Now open the assembly with options as shown below in the image.

We can now see the mates in the Feature Manager tree similar to the resolved mode. The assembly is still loaded in the graphics mode only. We can edit the supported mates, add new mates , delete mates etc. as if the assembly is loaded in resolved mode. Not only this, we can now save the assembly after mate operations and if assembly is open resolved, we can see the changes saved. The movement of components including pattern components is similar to resolved mode and much, much faster.

Supported Mates

The supported mates are all the standard mates. Some advanced mates such as distance, symmetric and width mates are also supported. The entities supported are planar, cylindrical, conical faces, vertices, linear and arc edges. The reference geometry mates are also supported but are not editable. The unsupported mates are shown with a different symbol in FM tree as shown below in the image.

Also the components which have unsupported mates are temporarily fixed with a different symbol in the feature manager tree as shown in the image below.

In addition to the above open any part from the LDR assembly through options on RMB in the FM tree on the component. Make changes to the part (for e.g. delete faces, change dimensions, etc.), save the part and switch back to the top assembly; the changes will be seen in the LDR assembly and also the mates related to the changed part will be affected. Similar affect when we change configuration of the graphics component. All very fast…

Published References and Magnetic Mates

The published references in SOLIDWORKS 2019 can now be visible in Large Design Review with edit assembly mode. We can now see the Published references in the Feature Manager tree. In addition to this connection points are visible in graphics area. The existing magnetic mates can be solved, new magnetic can be created/deleted, locked /unlocked. Ground planes can be edited/created all very fast because every component is in graphics condition only.

Additionally any changes to the connection point definition in the referenced documents can be handled in the LDR assembly. Also when a new part or assembly in graphics mode having published references is inserted in the LDR assembly, the magnetic mate is created similar to the resolved case and again all very quick.

Known issues in SOLIDWORKS 2019 B1

1. Property manager does not show mates of a graphics component on LMB.
2. Mates do not fail/update in top assembly when a graphics component is open resolved, changes are made to the component in its own window, saved and switched back to the top assembly.
3. Mates do not update in top assembly according to the configuration changed of the graphics component.

Limitations

1. Flexible assemblies are not supported. This is because the mates of the flexible sub assemblies are not loaded. They are still in in the graphics state.
2. The mates of the sub assemblies are not supported because the sub assembly is in the graphics state only.

Behind the screen

Well, how it is exactly implemented? The identification of the faces (face IDs), edges (node IDs) and the vertices are used to get this working while editing assemblies in LDR mode. These IDs are persistent both in resolved as well as LDR mode.   I can give you an example. The user selects a first face (say planar face) of a component of assembly.  A first reference plane is then created, in memory, and the face ID and/or edge IDs associated with the first face are stored as being associated with the first reference plane.  The reference plane can be defined by a point on the plane and the “normal” to the plane.  The face ID may include all nodes that are part of the first face, the edge IDs may include pairs of nodes, which can be obtained from the component entity information stored for the model.  The user then selects a second face in the assembly.  A second reference plane is then created, in memory, and the face ID and/or edge IDs associated with the second face are stored as being associated with the second reference plane.  The user may then add a constraint between the two selected faces by, for example, selecting a constraint type from a list of available constraint types for the two components (e.g., coincidence constraint, parallel constraint, etc.).  Constraint information is created and stored, temporarily, when in large design review mode. The user may add additional constraints in the same manner.  The constraint information can be saved in the constraint data stream for the assembly if the changes made while in large design review are saved.  The constraint stream can include a number of constraint entries.  A constraint entry can include information such as, for example, constraint type and entities associated with the constraint.  An example constraint entry can include:  an identification of a parallel constraint and an identification of two faces of the assembly, along with associated node information. In similar when a resolved assembly saved in SOLIDWORKS 2019 is edited in LDR mode, the information stored related to faces, edges, and vertices (IDs) are used to form geometrical entities which are further used to solve the constraints similar to resolved case but much faster.