Drafting Detail view Boundary 1

[Mitchel123]

Hi,

Please see the attached picture.

When selecting 'detail view' option in drafting, from the drop down menu the only option available is circular , rectangular by corner etc but if you look at the attached picture the circular 'detail view' was selected but the detail C has no circle and it has different outside boundary.

Please suggest a possible way of doing this.

The picture is created manually for explanation purpose

Thank you

regards

Mitchel

 

[JohnRBaker]

What version of NX are you using?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Mitchel123]

NX 8

 

[SvenBom]

1. click on the view with right mouse button (RMB) and select Activate Sketch
2. now, draw a spline in this view. Draw the open spline (not closed!) from one edge to another.
3. finish the sketch
4. now, click again on this view with RMB and select Add detail view.
5. select whichever you want, circular or rectangular. Just make the detail big enough to enclose the previously drawn spline.
6. place the detail view
7. now, click on detail view with RMB and select View Boundary
8. in new dialog box, select Break Line/Detail, then select the spline (in detail view) and click apply
9. new line Will apear. It Will connect both ends of the spline.
10. click on this line and move the cursor. The boundary line Will deform. Click again, to define new boundary. If you need some more modification, click again on the line.
11. click OK to close the View Boudnary dialog box.
12. hide all sketches. This Will hide the spline, that you have creatd in the step 2.

I will also attach the movie, for better understanding.

REgards.

 

[SvenBom]

Here is the movie, that I promised.
Regards.

 

[JohnRBaker]

Do you mean like this:

If so then after creating the Detail view, select this new view, press MB3 and select the 'Convert to independent Detail'. Now go to...

Edit -> View -> View Dependent Edit...

...and select the Detail view, select the 4th icon, 'Edit Object Segments', in the 'Add Edits' block, change the 'Line Font' in the 'Wireframe Edits' block to 'Invisible' and then hit Apply. Now follow the Que/Status line instructions, first selecting the view boundary curve, then two curves that define the start and stop of the segment to be 'removed', select which of the two segements you're 'removing' and then hit 'Back' and then OK and you should have your trimmed detail view. If you also wish to change the font of the View Boundary you can do that either by changing the Curve Font to Solid in View Preferences before creating the Detail view or by selecting the view and editing it's 'Style' changing the boundary from 'Phantom' to 'Solid'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[JohnRBaker]

Well, if it's a movie that you want, here's a video showing my proposed workflow.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Mitchel123]

Thank you John and SvenBom.

SvenBom I am unable to see the video properly, the working area is displayed with NX Welcome page.

Also John, I think the picture I have attached now can explain clearly what I am looking to do. Although what you have explained in the last video was also pretty useful. Please do have a look at the attached picture.

Thank you

regards

Mitchel

 

[JohnRBaker]

OK, after creating the normal detailed view and after selecting the 'Convert to independent Detail' option, as described in my post above from Thursday, just follow the workflow shown in the attached video.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[SvenBom]

Sorry for uploading such a dumb movie.
Here is another one.

Hope, this one Will help.

 

[Mitchel123]

Thank you John and SvenBom. You guys are great.

Can you please direct me to any tutorials or forum available to learn working with Layers? I have never worked with layers before.

Thank you

regards

Mitchel

 

[JohnRBaker]

This is only my own personal opinion, but if you've managed to live this long without learning a lot about layers, you can probably continue without losing any sleep over the idea that you haven't taken enough time to learn more about them.

That being said, while it is true that NX still fully supports layers and there are a few things that can be done well using layers, for those of use who have been in this industry for a while (in my case, 37 years this coming August) the value of layers has diminished over the years to the point that there are other, more modern ways to control the display and accessibility of data and objects. And I suspect that to some extent, this will explain why you are going to be hard pressed to find a lot of material about how to use layers or at least nothing that is as modern as videos and on-line tutorials.

But if anyone wishes to disagree, please feel free, and if you have some material which you think is compelling in showing how Layers can be used to enhance the effectiveness of NX, lets see it, OK?

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[SvenBom]

There is really not much to learn about layers. In every NX part, you will have layers from 1 to 256. It is up to you, which of those will you use.
If you decide to use layers, then create some rules first. For example, layers from 1 to 10 will be used for solids, for 11 to 20 for sketches, etc. And use them like this all the time.
When you want to move some geometry to another layer, you are using Move to Layer command (or Copy to Layer, if you want to have the same geometry on several layers). In Layer Settings, you can define, which layer is currently the work layer, wich layers are selectable (you can see and select the geometry), which is visible only (you can see but you can not select the geometry) and wich is invisible (you can not see the geometry).

But, to control visibility of the feature, I think LAyers are not the best option. As John already mentioned, there are better ways.

The only time, that I use Layers are when I am in drafting.
You can control visibility of the geometry in drafting views with Show/Hide or Reference Set. But this will affect all views, not only one. With layers, you have another option. In drafting, there is option Layer Visible in View. With this option you can define, that one piece of geoemtry (datum planes, sketches, etc.) is visible in one view, but it is hidden in another.

This is quickly about layers. And this the one option of using layers, that I remember now.
I guess, that others will provide some other ways of using layers.

Hope, that this helps.

 

[JohnRBaker]

I agree that perhaps the most compelling use of layers in NX today would be to control the display of secondary geometric objects on a per view basis when making a Drawing, as described by SvenBom. Of course, with the advent of PMI and the idea of adding the non-geometric data directly to the 3D model and use of the Model views to control the display of the PMI objects, layers are reduced to an even more diminished role.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[Mitchel123]

Good explanation guys. I completely agree with you both but the fact is that my new Job require me work with layers as they have been using layers from day one and they want me to follow the procedure. I have never used layers before but trying to learn myself.

You are right SvenBom. I will be using the layers in drafting and we are currently working on a pretty complex assembly which require drafting for individual parts and layers will play vital role to show/hide the geometry.