Coordinate Systems Now Mightier Than Origins, Planes and Axes

This is the second article from the “Do You Believe in SOLIDWORKS 2022?” series, where we dissect the latest enhancements in your design software.

In the first article of this series, Fast Drawings of Slow Assemblies, we established the following criteria for judging if a new enhancement is eligible for the “I Believe!” pin:

  • Security. It should not introduce new bugs or regressions. If anything, the software should operate more securely than before.
  • Ease of use. SOLIDWORKS users expect their software to be intuitive.
  • Clear benefit. The new feature should eliminate limitations in functionality or increase productivity.
  • Wide use. The more use cases in more industries, the better.
  • Requested by users. Users get what they asked for.

A Revolution in SOLIDWORKS?

Digging deeper into the new release revealed a hidden gem—maybe the most important enhancement in the new release. It is the increased functionality for the coordinate system feature, which is also Nate Andrews’ first pick in his recent article about SOLIDWORKS 2021 posted on After attending several What’s New in SOLIDWORKS 2022 presentations delivered by Dassault Systèmes or by resellers, we did not notice a lot of excitement for this enhancement from the presenters. Also, there seems to be very little information about its use cases in the various blog posts that covered the launch.

The What’s New in SOLIDWORKS 2022 guide lists two areas where the coordinate system functionality has been improved:

1. Defining the location and orientation of a coordinate system. There are two new options:

  • Use numeric values for defining position.
  • Use numeric values for defining orientation.

Figure 2. New definition options.

2. Giving the user access to all components of a coordinate system for referring it in sketches, features and mates, including:

  • Origin
  • Axes
  • Planes

At first sight, the enhancement is good but nothing to write home about. Very few people would get excited about an improvement to such an abstract feature as the coordinate system.

But as we discovered new ways to incorporate the enhanced coordinate systems in various modeling workflows, we got more and more excited. Even the title of this article changed several times as we kept added more pages to its draft. This is a short list of the titles we considered:

  • Shrink the FeatureManager with the New Coordinate Systems
  • Freedom from the Tyranny of the Model Origin
  • 3D Sketching Simplified in SOLIDWORKS 2022
  • Another Tool for Top-Down Modeling in SOLIDWORKS 2022
  • A Potential Revolution in the SSP (Skeleton Sketch Part) Method
  • New Entities for Mating – 2022 Coordinate Systems

The only way to gauge the value of an enhancement is by looking at potential use cases that could significantly change the way designers are using SOLIDWORKS. We found several. So, instead of discarding these titles, we decided to keep them in the article and attach a different case study to each of them. We will judge the pros and cons using two criteria:

  • Functionality unlocked in SOLIDWORKS 2022.
  • Opportunities to further improve the tools.

A. Shrink the FeatureManager with the New Coordinate Systems

Users who create a lot of reference geometry features will be the main beneficiaries of the new functionality.

It is typical, especially for power-users involved in the conceptual phase of a new design, to create multiple planes, axes and reference points early in the FeatureManager tree. The main goal is to reduce dependencies between the various sketches and features in the model, so that when needed they can be easily modified or even eliminated with minimal impact on the rest of entities in the model. Since reference geometry features have a minimal rebuilding “cost” they are usually used intensively in such a workflow.

In Figure 3, there is an example of a traditional reference “scaffolding” created in a part file, where the origin and the major planes are not in a usable location. The user requires “translating” the reference frame:

  • 3” in the “Y”-direction
  • -4” in the “Z”-direction

and to rotate it by -30˚ around the “Z”-axis.

Figure 3. Eight features are seven too many. I am getting a headache just by contemplating to work with such a “busy” graphic area.

In this example, the required reference geometry is composed of seven features:

Base Planes (1, 2 and 3) – usable for:

  • Creating sketches.
  • As references in sketch relations.
  • As references for defining coordinate systems’ direction.
  • As references for establishing feature direction in Patterns, Extrude-Boss, Extrude-Cut and Move Face.
  • Caping cavities using Intersect.
  • Splitting features.
  • As references for mates.
  • As Ground planes for facility layouts.

Ref Axis (1, 2 and 3) – usable:

  • As references in sketch relations.
  • As references for defining coordinate systems’ direction.
  • As references for establishing feature direction in Patterns, Extrude-Boss, Extrude-Cut and Move Face.
  • As references for mates.

A reference point named Locator – usable:

  • As a reference in sketch relations.
  • As a reference for defining location for coordinate systems.
  • As a reference for mates.

Even though the user took the time to name each feature, there is still a lot of clutter in the FeatureManager tree, and especially in the graphics area. Considering that such a part could be the main reference in a project, a user can spend a lot of “quality time” with it. He or she would need to repeatedly:

  • Find a specific reference geometry feature.
  • Select it (for the use cases listed above).
  • Control its visibility (hide/show).

Fortunately, in SOLIDWORKS 2022, all these features can be reduced to one – a coordinate system.

First, let’s define its position and orientation using numerical values.

Figure 4.

Then let’s compare the two parts side-by-side:

Figure 5. A reduction of 8 features in the FeatureManager tree.

The benefits are clear:

  • No clutter in the graphics area.
  • Easy visibility management (hide/show one item only).

Now let’s stress-test the functionality of the new coordinate system and propose future enhancements when needed.

Test #1: Selecting a Plane belonging to the Coordinate System in Part Mode

Figure 6. Context toolbar after a coordinate system plane was selected.

The context toolbar reveals that in part mode we should be able to:

  • Create a 2D sketch on any of the three coordinate system planes.
  • Orient the viewport normal to the coordinate system plane.
  • Create an offset plane based on the selected plane.
  • Measure from the plane.

Let’s test these four assumptions, as well (figures 8 to 10).

Figure 7. Usage as a sketch plane, Check.

Figure 8. Viewport orientation. Check.

Figure 9. Use in defining new planes. Check.

Figure 10. Measurement to another plane. Fail.

As shown above, currently (SOLIDWORKS 2022 PR1) when attempting to measure the angle between a coordinate system plane and another plane it intersects, the result is meaningless. There is no angle reported, only the distance between the coordinate system origin and the second plane.

We will report this limitation to SOLIDWORKS and hope to see it fixed soon.

Test #2: Selecting an Axis belonging to the Coordinate System in Part Mode

Figure 11. Context toolbar after a coordinate system axis was selected.

The context toolbar reveals that in part mode we should be able to:

  • Orient the viewport normal to the selected axis.
  • Measure from the axis.

Let’s test these four assumptions (figures 12 to 13).

Figure 12. Viewport orientation. Fail.

When an the Normal to is applied to a selected axis, the viewport is oriented based on the default triad and not normal to the coordinate system axis. Another opportunity for a future enhancement.

Figure 13. Measurement to plane. Fail.

Same behaviour is observed here, too. The Measure tool needs to be recoded to recognize the components of the coordinate system.

Conclusion – Shrink the FeatureManager Tree

For users who build complex models, this enhancement will be a game changer. SOLIDWORKS 2022 delivered a vastly improved tool that offers huge benefits:

  • Drastically reduce the length of the FeatureManager tree.
  • Declutter graphics area.
  • Save time during conceptual phase.
  • Huge time savings for revisions.
  • Decrease the possible sources of errors.
  • Eliminate the occurrence of dangling entities after revisions.

B. Freedom from the Tyranny of the Model Origin

One of the first lessons SOLIDWORKS users learn is to take advantage of the origin to locate sketches and features. You cannot change the origin; if you need to move the part, you can use the Move-Body feature, or attempt more convoluted workflows such as:

  • Inserting a part in another part and re-positioning it.
  • Create a coordinate system in the desired location for the new origin, save the file to Parasolid with that coordinate system as the origin (of course, losing all features in the process) and re-import it in a new part.

When users ask us the simple question “How do I change the origin?” we used to encourage them to accept the established paradigm.

But what if we were to model the part in regard to a coordinate system instead of the main origin?

In Figure 14, there are two SOLIDWORKS 2022 sessions shown side-by-side, each of them containing apparently similar models.

Figure 14. Freedom from the origin.

The difference is that in the model on the left, many of the sketches and features are related to the origin and/or the major planes. Editing these features to reposition or reorient the model is next to impossible.

The model on the right contains the exact same features. The only difference is that instead of referring the origin and the major planes, the sketches and features are referring to the planes of the coordinate system 1. Now, let’s see what happens if we modify the position and orientation of this coordinate system.

Figure 15. Simply edit the coordinate system definition.

Figure 16. The model has been re-positioned and re-oriented with ease.

The result is spectacular. This is what many users have been asking for a long time and now SOLIDWORKS has delivered.

Considerations for successfully using this technique

  1. If the users foresee that the model might require re-orientation (rotations) then they should refrain from using Horizontal and Vertical sketch relations, since such relations are referring the default triad. Use instead Parallel or Perpendicular relations to the coordinate system planes
  2. At this time, you cannot refer the origin of the coordinate system in sketch relations or dimensions. The workaround uses Coincident relations to the coordinate system sketch planes.

Conclusion – Freedom from the Origin

SOLIDWORKS finally found a valid answer to a question asked by many users. While users must be diligent in applying the right relations when creating sketches, this is not hard to do.

The result is spectacular and could drastically simplify or even eliminate cumbersome workflows used by many companies.

C. 3D Sketching Simplified in SOLIDWORKS 2022

Working with 3D Sketches can be time-consuming and cumbersome, mostly due to the need to create and manage a large number of sketch relations.

It is not uncommon for a 3D Sketch to have a larger number of centerlines and reference planes, than the actual number of useful entities (lines, arcs, circles).

Considering that just one coordinate system contains a reference point (its origin), three axis and three planes, the new functionality could be a game changer for users by drastically reducing the number of centerlines and 3DSketch planes needed.

Let’s stress-test this functionality. Using the same part shown in Figure 4, we added a 3D Sketch.

3D Sketch Test #1: Add Relations between a Line and a coordinate system Plane

Figure 17. Possible relations between a Line and a coordinate system plane.  Check.

As shown in Figure 17, there are some very handy relations that can be added and work as expected:

  • Horizontal to the plane (which also means that the line is On Plane).
  • Vertical to the plane (which also means that the line is On Plane).
  • Normal to the plane.
  • Perpendicular to the plane (similar to the previous relation).
  • Parallel to the plane.
  • On plane (coincident to the plane).

The other two relations that are shown as available in Figure 17, (Parallel YZ and Parallel ZX) unfortunately are being applied to the default triad directions, not to the coordinate system (Figure 18).

Figure 18. Parallel YZ and parallel ZX. Fail.

Again, we will report this unexpected behaviour to SOLIDWORKS.

3D Sketch Test #2: Add Relations between a Line and a Coordinate System Axis

Figure 19. Attempting to add relations between a line and a coordinate system axis. Fail.

When selecting a coordinate system axis and a line, we get the same icons as when selecting the plane. At this time, we recommend users refrain from applying such relations because they produce wrong results (example in Figure 20).

Figure 20. Unexpected result when trying to make the line parallel to the X-axis of the coordinate system.

3D Sketch Test #3: Add Relations between a Line and a Coordinate System Origin

When selecting a line and a coordinate system origin, there is no usable relation available (Figure 21). One would expect just a coincident relation to appear in the context toolbar, but currently that its not happening.

Figure 21. Relation between a line and coordinate system origin. Fail.

Conclusion – 3D Sketching and Coordinate Systems

The limitations related to referencing coordinate systems axes and origins will most likely be fixed in one of the upcoming service packs. Even if users would use only the existing functionality of applying relations to the three coordinate system planes, they could drastically reduce the complexity of their 3D Sketches, decluttering the graphics area and decreasing rebuild times.

D. Another Tool for Top-Down Modeling in SOLIDWORKS 2022

One of the main challenges that users encounter when performing top-down design is managing references.

When vertices, edges and faces that are referred to by other components are drastically modified or deleted, these references dangle, generating a lot of confusion and frustration. A huge amount of time is lost with such errors occurring every day.

Imagine how much easier the work could be if users would add one small step to their top-down workflow: create most of the relations between parts using coordinate systems.

Of course, not every external relation can be created using the new functionality, but many could.

Suggested Workflow

  1. Edit the “child” part in the context of the assembly.
  2. Add a coordinate system inside this part with a position and orientation defined by the entities from the assembly.
  3. Open the part in its own window.
  4. Add new features as needed in relation to the new coordinate system.

If the parent components are edited, the worst thing that could happen is for the coordinate system to lose some of its references. Fortunately, redefining it is very simple.

Conclusion – Another Tool for Top-Down Modeling

Top-down modeling should be performed by properly trained users. The success of this method lays mainly in managing the number and complexity of the references.

Ideally, the length of the chain of dependencies should be minimized (ideally a one-step dependency). Until now the ultimate dependency simplification could be achieved using a combination of sketches, planes and axes. Starting with SOLIDWORKS 2022, users add one more super-tool to their arsenal, a tool that combines seven other tools in one (origin, three axes and three planes).

E. A Potential Revolution in the SSP (Skeleton Sketch Part) Method

In essence, the SSP is one of the most solid methods that could be used for managing a huge number of parts and assemblies with zero relations between them.

In its purest form, the SSP creates assemblies with zero mates and no external relations between components, other than the relation between the base part and each component of the assembly (part or sub-assembly).

We are currently evaluating the potential to introduce the newly enhanced coordinate system feature in the SSP workflow and the preliminary results are very good.

The SSP is such a vast topic that it deserves its own series of articles. Stay tuned for that.

F. New Entities for Mating – 2022 Coordinate Systems

Coordinate systems have always had super-powers when used in mates. They act as origins, allowing the same freedom for defining only position, or also orientation.

SOLIDWORKS 2022 makes them much more powerful than the default origins. We can now mate to each of the three coordinate system planes and its three axes.

This part of the enhancement was perfectly implemented by SOLIDWORKS. While stress-testing it, we could not find any flaw. Take a look at the following examples:

Figure 22. Planar Face and coordinate system plane – Quick Mate toolbar.

Figure 23. Coincident Mate applied.

Figure 24. Cylindrical face and coordinate system plane – Quick Mate toolbar.

Figure 25. Distance mate applied between cylindrical face and coordinate system plane.

Figure 26.  Coordinate system axis and cylindrical face – Quick Mate toolbar.

Figure 27. Concentric mate.

Figure 28. Select the coordinate system points to replicate the old functionality for mating two coordinate systems.

Figure 29. Coincident mate between coordinate systems axes.

Figure 30. Parallel mate between coordinate systems planes.

Current limitation

Coordinate System Planes cannot be currently used in defining ground planes for facility layouts.

Conclusion – New Entities for Mating

Allowing users to mate to any of the seven components of a coordinate system unlocks a lot of opportunities for simplifying the mating scheme and saving time. The user now has the choice between eliminating three, four or all six degrees of freedom, using coordinate systems.

Final Conclusion

When a feature such as the coordinate system receives such a major update, it is expected that improvements will be added in multiple phases, over several releases. SOLIDWORKS 2022 simply unlocks functionality that users requested for a long time, making their life easier in all modeling environments:

  • Sketch
  • Part
  • Assembly

Suggestions for Future Improvement

1. Allow users to apply colors to the coordinate systems. That would dramatically improve their visibility on the graphics area.

Figure 31. Colors will be a game-changer for managing the reference geometry in the graphics area.

2. Make dimensions used in defining coordinate systems visible, selectable and editable in the graphics area. That would drastically improve user speed when revising the model.

Imagine, if you could, simply double-clicking on the coordinate system and its dimensions would pop-up on the screen. Then double-click any of them to edit.

3. Allow the numerical values used in defining coordinate systems to be driven by equations, custom properties or design tables. Adding this functionality will further enable users to automate their design.

4. Allow coordinate system planes to be used in the definition of the intersect feature.

5. Allow the patterning of coordinate systems.

With the expectation that the new enhancement requests listed in this article will be implemented soon, we decided to wear the I Believe pin.

Let us know what other topics you would like to see covered in the I Believe in SOLIDWORKS 2022 Series.

Learn more about the new enhancements in SOLIDWORKS 2022 with the eBook SOLIDWORKS 2022 Enhancements to Streamline and Accelerate Your Entire Product Development Process.

About the Author

As an Elite AE and Senior Training and Process Consultant, working for Javelin Technologies – a Trimech company, Alin Vargatu is a Problem Hunter and Solver.

He has presented 31 times at 3DEXPERIENCE World and SOLIDWORKS World, once at SLUGME and tens of times at SWUG meetings in Canada and the United States. His blog and YouTube channel are well known in the SOLIDWORKS Community.

In recognition for his activity in the SOLIDWORKS Community, at 3DEXPERIENCE World 2021, the SWUGN (SOLIDWORKS User Group Network) awarded the SOLIDWORKS AE of the Year title to Alin Vargatu.

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