Connect Views w/ Chain lines 1

[DaSalo]

Hello,
NX 6.0.5.3 drafting:

I'm new to NX drafting and am trying to create a print with several auxillary views projected at non-orthoganal angles. I figured out how to specify the vectors by choosing two points in the part geometry but now I would like to connect the new views to the base view with chain lines so that the reader can more easily follow the projections. Anybody have a good technique for creating lines that relate one view to another? I see this done all the time on GE prints but so far haven't been able to figure out a good method.

Thanks

 

[uwam2ie]

... do a training on NX

 

[DaSalo]

Nah, I figured it out. Just took some playing around and I was hoping someone would have some helpful advice.

Thanks

 

[cowski]

It would be helpful if you post the solution you found. That way when someone searches the forum in the future they will find an answer.

 

[DaSalo]

Cowski,
Happy to post my solution. As mentioned previously, I am new to NX drafting so there might be a much better way to do this. See attached JPEG for an example of the effect I am trying to create. I am not sure if this is proper drafting practice according to any standard; it is something I have seen from several designers that I have found useful when inspecting parts both on the surface plate and CMM.

The problem:
The part has surfaces that are at compound angles relative to square surfaces that will be used for datums. Orienting to these surfaces requires either a compound sine plate setup or multiple coordinate system rotations for the CMM. Sometimes it can be very difficult to trace the progression of rotation of the auxillary views on the print. This is especially true if there are many surfaces with dozens of auxillary views on the page or when angles are only a fraction of a degree off from true orthographic angles.

A solution:
It can be very helpful to the print reader to visually connect the auxillary projections in sequence so they can immediately grasp how the part or coordinate system will need to be rotated to orient to the feature in question. It might be possible to generate these connecting lines by expanding the view and sketching them in within the drafting module but I found it to be much easier to do this in modelling. I created a seperate layer for drafting specific objects and then added the lines that I needed using the "Curves" toolbar. I used the "Edit Object Display" tool to change the lines to a phantom line type. I also used "Move object" to move the line off the part to establish a reasonable looking gap.

Once I had all of the lines I needed I went back to drafting, turned on my drafting objects layer in the views that it was required, and edited the view boundary using "manual rectangle" to overlap one view onto the next so the line appears to be connecting the views. It is helpful to make the lines very long when creating them in modelling so that you will have plenty of flexibility to move the views apart until they all fit nicely on the page. I then used "View Dependant Edit" to delete all but the one line that I needed from each view.

Once the lines are on the page you can dimension to them to call out the rotation angles. It might be better drafting practice to add additional phantom extension lines to use for dimensioning instead of dimensioning directly from the part as I have done in my example image. That way it would be clear that these dimensions relate to the views themselves and are not being used to directly dimension a part feature.

That's about all. Any suggestions on an easier way to do this in the softare, any thoughts on alternative approaches to this type of drafting situation, or any other thoughts much appreciated.