dimensions from centrelines

[bengee5454]

why oh why can I not create angular dimensions from centrelines?

Working on dwg of a complex pipe model and I want to take all dimensions from centrelines.  I select the centrelines (to give an angle), but no dimensions appear.

Frustrating does not even come close! 

[JDMather]

Works for me?

What version of Inventor (including, of course, Service Pack and/or Update information)?

Can you attach example files that exhibit this behavior?

[rhasell]

Hi

Have you tried changing the "Dimension Type" of Projected/true?

[bengee5454]

This is the drawing I'm currently working on.  For example, I've been trying to dimension the right hand branch angle (lower left view). I've shown it marked in red as 42°. I obtained this dim by selecting the outer edges of the pipe. I really want to be selecting the centrelines.

I have dimensioned from centrelines elsewhere, but i've had to create a sketch on that view, and dimension from the sketch....then hide the lines. Obviously not ideal!

[bengee5454]

I'm using Inventor 2014 SP 2

[TheCADWhisperer]

Did you Retrieve all of these from model?

I noticed that it was one continuous entity - cannot select the same entity twice for dimension.

If I delete the centerlines and add them manually - I can then add the dimension.

Edit: Wait a minute - I see what you did.  You did these centerlines as view sketches.

You don't need to do that.

Simply select the Centerline Bisect and the edges of the pipes.

Now you can dimension.

[bengee5454]

For instance, I cannot seem to pick the 2 centrelines of the dimension (shown in magenta)

[TheCADWhisperer]

Works fine here - if I use centerline bi-sector rather than a view sketch.

[shiyong.lin]

Did you create the continuous centerline from "Automated Centerlines..."? The automated centerlines contain multiple line segments, you cannot dimension angle between two coninuous centerlines because Inventor doesn't know which centerline segment is used for measuring the angle.

As several other people mentioned already, the best way is to create bi-sector centerline for your dimension needs.

Shiyong

[rhasell]

Hi

In a nut shell to put everyone's comments plainly.

STOP sketching in your centrelines. Delete the existing sketches as they are affecting the dimensions.

[bengee5454]

I only created the sketch centrelines because I couldnt select the true centrelines. The drawings were needed immediately, pressure was mounting, and as I couldnt create a 'normal' dimension I had to create a quick fix.

Dont get me wrong, I make no habit of doing this! 

[TheCADWhisperer]

---

@Anonymous.gee wrote:

..., pressure was mounting, .... I had to create a quick fix. 

---

Do you understand the correct technique now?

I ask, because you posted this same question even after the solution was given earlier.

The correct technique is much quicker.

[rhasell]

Hi

If you really need to sketch the centerlines, there are a few more 'Stable' methods.

One option is to retrieve the dimensions from the part, even if you have to create an additional sketch in the part to accomplish this. This is far more accurate for what you are trying to achieve, as I have found that I will get conflicting results depending on the type of dimension and view orientation.

To have fixed your immediate issue, multiple sketches would have been required, one for each centerline, or alternatively just the centeline sketch for the individual section required for the dimension value.

You could also place the dimension in the DWG sketch, and use the retrieve dimension option, that way you don't need multiple sketches.

I personally have to sketch in centerlines occasionally as the Centerline bisector fails and will not generate a CL. In my case, it is normally a detail view of a Rolled CHS, my assumption for the CL bisector not working, is that there is not enough information on the view to create a centerline.