Why does Onshape not show centerlines associated to cylindrical surfaces in the 3D model?

It would be nice if there was a way to move a "Discussion" to another category instead of reposting it.

I think it is a little premature to make it an "Improvement Request". It is entirely possible that my lack of experience with the product is the problem. I think it would be appropriate for others to comment (attempt to answer the question) and/or confirm that centerline display for cylindrical surfaces is something that should be addressed. 

Never having been a SW user I am not familiar with the term "temporpary axes".  I disagree that adding a "Mate Connector" to the model addresses the issue, in fact it makes things worse.

When I see a "Mate Connector" (MC) I am going to assume the designer added it specifically to denote that the feature geometry it is associated with exists to support a mating relationship with another part. The MC is there to communicate this feature surface "touches" something else and to facilitate the assembly to another part in the assembly tool build process. Adding a mate for any other purpose should be discouraged.

Using a "MC" to denote a surface is the result of a revolve/arc extrude does not address my issue with creating feature sketch alignment to a feature that does have enough geometry to derive its centerline. I need to be able to do a "Project" select a revolved or extruded arc surface and at least have the option of getting its centerline/axes as well as its silhouette edges. The "Project" command does not recognize a MC so it is useless to me for that purpose.

I agree that arbitrarily displaying centerlines for every feature/surface, that might have one,  can clutter up the display making 3D viewing more difficult. That is why I mentioned that there needs to be a simple method to control (turn on/off) the display of centerlines at the feature/surface level; I only want to show the ones that affect the functional parts of the design.

Besides Planes, adding the ability to create 3D points, 3D lines, and 3D Coordinates Systems as supplemental geometry in a Part-Studio (even an Assembly) would go a long way to addressing the need to be able to design at a more abstract level and represent/flag key aspects in the model. 

Here is the information you requested...

First, I am going to have to retract what I said about “in some cases [it is] impossible” to derive a centerline from the geometry; it is always possible even though the steps required to achieve it can be tedious.

My two arguments for getting access to and having “3D centerline” display for geometries that have them (extruded 2D arc/circle, any surface created via revolve and a sweep path) are:

1) The display of 3D centerlines quickly communicates to the observer important information about the function of and construction methods used in the model. Features with a centerline are often the most critical features in the model relative to the modeled product's function and having them displayed makes the process of understanding what the model is all about quicker.

This argument alone should be sufficient to warrant display of 3D centerline in the model.

2) It is common practice to create secondary features that need to maintain alignment with a centerline of an existing feature.

I will use the time honored model of a block with a hole to make the point…

The design requirement is to create a hole feature that maintains alignment with the existing hole feature in the block. (I will not attempt to explain the “real world” purpose of the feature, but trust me, it is a very common feature-to-feature relationship.)

Since the 3D centerline of the existing hole feature is not accessible it has to be derived from what geometry is available. For this simple prismatic model a couple of methods exist:

“Use” (project) the circular edge onto the sketch plane as a construction curve. Draw another construction curve that represents centerline making sure it is midpoint and perpendicular constrained to the projected curve. This is by far the simplest method; however, it makes all sort of assumptions about the parent hole feature. It only works if the circular edge accurately represents an edge that is perpendicular to its centerline axis.

Also, one must be very careful using implied sketch constraints to make sure the constraint relationships are created between the correct curves. In the above the projected circle edge happens to superimpose a sketch edge associated to the block geometry. It would be very easy to create both the midpoint constraint and perpendicular constrain to the wrong curve.

A more robust approach would be to project the hole’s top and bottom’s edge curves and sketch a construction line between the midpoints of the curves.

The other method “Uses” (projects) the face/surface of the hole to the sketch plane; the result is two parallel lines from which an additional construction line can be sketched and constrained to be symmetrical to the projected curves.

Again, you must be very careful sketching the construction line that represents the centerline. Highly recommend sketching with “sketch inferences” turned off (depress and hold down the <Shift> key during the sketching process) so that you observe the sketched line snap into place centered between the two projected curves when applying the symmetry constraint.

Note: The “Used” and my “centerline’ sketch curve end points are not constrained (I didn’t feel like adding 6 coincident constraints). I know the line lengths are not important relative to maintaining the aligned condition. However, the end points should be constrained for the benefit of the person who might look at this sketch in the future; it would be difficult to interpret if the construction lines wandered way off the geometry.

The last two methods are far more robust because the hole surfaces can be cylindrical, or conical, any any orientation in the model (the exception being when the centerline is normal to the sketch plane).

All the above techniques are dependent on seeing the “holes” surface trim curves, or silhouette edges that represent its true size as viewed from the orientation of the sketch plane.

If you do not have this condition the process to derive a centerline is more tedious. For example:

“Use”ing ether the curve edge of the cylinder, or its surface doesn’t produce enough geometry to derive its centerline.

In my limited experience with Onshape I have yet to encounter this situation, but if I did I would find the pertinent sketch(es) that produced the feature with a centerline and if necessary supplement them with additional curves, make that sketch visible while sketching the curves to create my aligned feature and “Use” (project) the needed curves.

An additional construction line was created constrained parallel to the projected cylinder silhouette edge and coincident with the endpoint of the projected supplemental arc from the sketch used to create the cylinder feature. Now the construction line representing the centerline can be created and constrained to be symmetrical between the 2 lines representing the feature’s silhouettes. Again, one needs to pay very close attention during the sketching/constraining process to make sure you properly capture/express this design intent.

For feature geometry created with the revolve command I would probably go to the sketch where the profile was created and there hopefully find the curve representing the axis of revolution.

I hope you appreciate how tedious and error prone the process can be compared to how simple it would (should) be if the 3D centerlines existed.

I trust my two arguments for displaying and providing a more direct means to access the centerline of features are sufficient to make adding display and access to 3D centerlines worthy of consideration.

I am happy that others have chimed in to discuss this subject, but I will not be happy until I see selectable 3D centerlines in the model.

I get a sense that my two arguments for having 3D centerlines are not sufficient justification to make an "Improvement Request". 

I am still very adamant about NOT using a Mate Constructor (even if it could be used as coordinate system) as a solution. It is a band-aid; an ugly band-aid.