reference dimensions using push/pull

[Anonymous]

There are times when I want to use the push/pull tool to change the diameter of a hole or thickness of a wall. However, I am only able to see the change in distance of the surface being pushed or pulled. I want to be able to see the total diameter of the hole or thickness of a wall as I am changing it. Is there a way to do this? Such as adding a reference dimension to model geometry that changes with the geometry?

[chrisplyler]

Ahem....

What you should do is stick some dimensions on some stuff, and then push/pull some stuff, and experiment to see what happens. That will definitely work. Plus you don't really want to do what you want to do.

(Not really. Just ignore the above. This is an undercover post to bait out @TrippyLighting  and see if he is watching me.)

[TrippyLighting]

Yeah man, one cannot be careful enough around here :

via GIPHY

[jeff_strater · Accepted solution]

well, one of us ought to try to answer @zero1991HJ2AC's question...  I think I understand what you are asking.  Take a look at the video below to see if that helps.  The key is the "re-anchor" tool inside of Press/Pull.

Jeff

[Anonymous]

The re-anchor tool looks like just what I need for flat faces. However, when I use press/pull on a cylindrical face, it does not give me the radius. In fact, I see on your screen that the manipulator arrow starts at the center. But when I select a cylindrical face, the arrow starts at the wall. I included a picture of what I mean. 

[Anonymous]

I just watched another video and realized that there is a difference between parametric environment and direct modeling environment. When I turn off the design history, the press/pull tool gives me the radius of the cylindrical face. So is it the case that the only difference between parametric and direct modeling environments is whether the design history is being captured?

[TrippyLighting]

It would provide some better context if you could let us know what other video you watched.

Parametric means that you can edit a sketch, or feature in the timeline and update it's parameters, like a dimension in a sketch or the length of an extrusion feature in the timeline. All that is captured in the parametric history. When you change that parameter the timeline is reevaluated and your design us updated and not reflect that changed parameter.

In DM mode that does not happen. If you change ht dimension is a sketch nothing updates except that sketch, but not the extrusion you might have created from that sketch. You can delete that extrusion and make a new one from the changed sketch.

Hopefully that explains the difference better between DM and TL mode.

[jeff_strater]

Yes, it would be helpful to see the actual case you are dealing with.  However, it is worth mentioning that Press/Pull in a parametric document is...  complicated.  Overly complicated, IMO.  The default, when selecting a face to Press/Pull, is to do a "smart" Press/Pull (I will try to withhold too many editorial comments about this "smart" mode).  In this mode, Press/Pull tries to figure out whether the face can be moved by editing the feature that created it.  So, if you pick a face created by Fillet, it will dump you into editing the fillet feature that created it.  If you pick a side face of an Extrude, then what is really happening is you are dragging the sketch curve on which that face is based.  If you pick the end face of a distance Extrude, then you are editing the Extrude distance.  If it cannot move the face by editing a feature or sketch, then Press/Pull defaults to creating a new Offset feature.  The Offset feature does measure distance relative to the starting point.

So, whether you get the new Offset, or some other version of Press/Pull is case-dependent.  So, seeing your data should allow us to offer a better explanation of what you are seeing.

[genopsdir]

Exactly the answer I needed! Thank you for sharing!