Dimension about center line

[Anonymous]

Can we get the option to dimension about the center line/construction line?

This would be especially very useful when drawing sketches for geometry that is going to be revolved around its center line. As the user would be able to enter in the desired diameter rather than having to calculate the radius.  

[David_Early]

DanSolo,

I think that functionality is already there.

In the sketch enviroment you have 3 types of line and you can combine the types.

Regular line: the line is for further use in features

Construction line: just for constructing the sketch, not possible to use this line in further features

Centerline: can be used as you discribe for revolved features, standard the diameter dimension is used around the center.

Try it out, functionality is ther and even more.

Greetings

[jtylerbc]

david.early is correct - Inventor sketches already behave this way.  You have to actually make the centerline a Centerline type though - just Construction lines won't do it.

[Anonymous]

thanks for that guys, it is a shame it has to be specific (for some unknown reason) but that answers that.

[David_Early]

What also works with any type of line: pick the dimension command, then pick your edges to dimension, (while the dimension is glued on you cursor click Right mous button and choose "Linear dimension". 

Greetings

David

[Anonymous]

thanks for all tips on how to make it work.

my observation as a user of both Inventor and SolidWorks and having read many of the posts on the Autodesk site. Is that yes there are ways to accomplish the same goal... and users as well as Autodesk software developers seem content with that. This is fine as long as your remain unaware of of the needless steps and effort to accomplish simple commands...commands that are often only single click or automatic functionality in other software. 

Autodesk Inventor has tons of these scenarios. And for users used to having rapid functionality, it is very frustrating. 

I intend to keep posting these little quirks and software deficiencies because I believe Autodesk Inventor has the potential to be better then most of its competitors. Its real power is its ability to be used in conjunction with other Autodesk software. But they need to make the software at least as good as its main competitor and they need to make sure they cover off functions and commands that have existed in competitor software for years. If a basic function can be done with a single click of a mouse and or provide more options, they need be at least as easy and fast.

[jtylerbc]

DanSolo, are you saying that all construction lines behave this way (automatic linear diameters) in SolidWorks?

If so, I would consider THAT annoying, just as you consider this Inventor behavior annoying.  In SolidWorks, what if you want to dimension directly from your construction/centerline to the second object, without getting a diametric dimension?  Not every construction line is intended to be a centerline for a cylindrical feature.  That is why there are two settings in Inventor (Construction and Centerline) that are seperate. 

As well, if you are going to use a Revolve feature, you really should be using the Centerline type anyway.  The Revolve command will automatically select it as the axis of revolution if you do. 

[Anonymous]

" In SolidWorks, what if you want to dimension directly from your construction/centerline to the second object, without getting a diametric dimension?"

Easy, simply moving your mouse past the centerline/construction line turns it into a diametric dimension... simple, quick.

As I use both, I can cite both Inventor advantages and Solidworks advantages in terms of functionality. However there are way more have-nots in Inventor, most of which are little, but make for a much easier time of modeling and a quick process to reach ones objectives. 

That said, as I mentioned beofre Autodesk Inventor has some other advantages that make it worthwhile. The downside unfortunitly is the the cumbersom modeling process itslef.

[jtylerbc]

That doesn't sound so bad then, and actually does have some slight advantage since it's not any more difficult to do the linear (non-diameter) dimension.  I wouldn't mind something like that as a shortcut for the second method that david.early described.  However, as I mentioned earlier, in Inventor there is at least one other reason to use the Centerline type.  If your requested feature existed, you could only make use of it by passing up that existing advantage (automatic revolve axis selection).

The buttons for Construction and Centerline are right next to each other on the ribbon.  In either the current situation or your proposed situation, you have to go click one of those two buttons.  To me, neither of these buttons seems harder to click than the other.  You're blurring the distinction between the two line types, but you're not getting away from the need to pick one of them.

Also, one minor gripe - at least according to the screenshot you posted, the SW linear diameter dimension doesn't show the diameter symbol (Ø).  Nitpicky, I know.

[Anonymous]

"one minor gripe - at least according to the screenshot you posted, the SW linear diameter dimension doesn't show the diameter symbol (Ø"

It does not have to be a center line at that point. For instance you can use such a dimension to layout a sketch that you are going going to mirror.

[jtylerbc]

Ah, I see.  So it's something like a Symmetry constraint without the need to draw the second instance.  In Inventor, I would see it being more useful for that scenario than for the revolve centerline scenario.  I see it as being less helpful for situations where the mirror is taking place in the sketch (in which case you can just dimension after the mirror), but it would be great for cases where the feature is going to be mirrored instead.

When you retrieve the dimensions into the SolidWorks drawing (assuming that process has a SW equivalent), can it tell which ones became diameters and which didn't, and add the symbol automatically when appropriate?  Technically Inventor can't tell the difference on its own, but the creation of the Centerline defines those dimensions as diameters, so they retrieve into the drawing with the symbol already placed.

[Anonymous]

"When you retrieve the dimensions into the SolidWorks drawing (assuming that process has a SW equivalent), can it tell which ones became diameters and which didn't, and add the symbol automatically when appropriate?  Technically Inventor can't tell the difference on its own, but the creation of the Centerline defines those dimensions as diameters, so they retrieve into the drawing with the symbol already placed."

To be perfectly honest, I am not sure.

I rarely use original model dimension in drawings, although I know some do and the option is there.

I prefer to add my dimemsions after as my model dimension typicaly define specific features as they are created rather than drawing dimension I am using to comunicate design intent and critical features, GD&T etc...

I will have to try it and find out.

[inv.ideareview]

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