A few questions with regards to NX8.5

[adam1986]

We have just migrated to NX8.5 and are trying to identify the following Drafting areas:

1. Can you dogleg /jog a dimension using a specific NX feature, rather than using a symbol or sketching as per previous version of NX

2. Are you able to edit a custom symbol once it has been created within NX. I created a custom table that had particular fields that needed to be filled in on input. I have noticed a mistake and can only find options to delete and redo all the field setting options.

3. What is the recommended method of dimensioning draft angle, ensuring it is associative to the model. Our current practice invloves manually typing the draft (Something when the model is updated the drawing is left at the incorrect draft). Our current process just involves tying +/-x` incl or similar and attaching it to the dimension. Other than using an expression (which is called up on every standard drafted surface) or having an angular dimensiosn on all the drafted features (which would be messy) I cant think of another way.

4. Is there a way of creating a double balloon (for sub-assembly identification) or will this need to be a custom symbol?



Thanks in advance for any help recieved,

Regards

Adam

 

[JohnRBaker]

I'm sure some actual users may also be chiming in here even if they're not on NX 8.5 yest since your questions are not version specific (or at least the answers shouldn't be).

As for 'dog-legging' a dimension, I'm not sure what you mean exactly. Could you provide a picture of what you're looking for? It will depend on what sort of dimension that you're talking about. For example, Ordinate Dimensioning as automatic dog-legging built-in.

As for editing a Custom symbol, generally speaking the symbol is considered a single object and so only things like embedded text or inherited text is accessible. The parts of the symbol itself are not. Now you can 'explode' a symbol which will convert it back into its basic lines, arcs, text, etc, which can then edited like any other wireframe objects, but it would no longer be a symbol. Generally the idea is that if you wanted a different sort of symbol you should create a new one and use it in the place of the one that wasn't quite what you were looking for.

As far as dimensioning 'draft angles', generally that's one of the reasons to create a section view of a model, since this will help make it clear that something actually is at an angle relative to some other part of the model.

And for grouping ID bubbles, once you've got the ID bubbles on your drawing just select the one that you wish to be the 'base' ID (the one with the leader), press MB3 and you will see that there are two options, 'Group Horizontally...' or 'Group Vertically...'. Just pick the desired scheme and then you will be asked to select the other ID bubbles that you want to group with this one and when you're done and you press OK, the selected ID bubbles and their leaders will be deleted and just the bubbles will be automatically recreated but now appended to the original ID bubble.

Anyway, that should answer some of your questions.

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.

 

[cowski]

There are a few different "divided" ID symbols that allow you to enter 2 lines of text (upper and lower text), is this what you mean by a double balloon?

www.nxjournaling.com

 

[adam86]

By double balloon I mean two concentric circles with a leader.

By Doglegged, I mean a Jogged dimension, ie to a point (ie split line) that could be hard to identifiy if the dimension was linear to the point, so is offset each side.

With regards to the symbol. I have created a table, which has locked fields and users are able to input data in each field as required. As i understand Johns reply, i would need to smash the the table, edit the text and recreate is as a symbol? This seems a bit excessive as there are over 40 fields to enter and select as editable/locked/etc?

 

[JohnRBaker]

Is the so-called 'double balloon' supported by any specific Drafting Standard?

This sounds like it might be something that could be addressed by a 'Narrow' dimension, but a picture of what you're talking about would be very helpful.

As for your 'table' symbol, have you looked at using a 'Tabular Note' instead?

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.

 

[adam1986]

Double Ballo Preview attached

 

[adam1986]

As far as i am aware, this is only a "company standard"
We currently use the standard single balloon, size 16, text 6, no jog/leader adn then sketch an 18mm circle around it.

I'm guessing creating a custom symbol is the way forward?

 

[cowski]

I'm guessing creating a custom symbol is the way forward?

Or lobby to change the company standard. I see no reason to use non-standard symbols that create more work for you and don't add any value...

www.nxjournaling.com

 

[kapmnit123]

Hi adam,
You can use custom symbols for editing the existing single circle to a double balloon symbol.Editing the master custom symbol is now quite easy as for editing a custom symbol you need not smash it just right click to edit the custom symbol and it will open the master copy for you.Make the changes and then come out of the edit mode.(However as John and Cowski already stated it is not be a good practise to fiddle with the existing standards and i totally agree with them).

As far as the table custom symbol is concerned so i will recommend use SAVE AS TEMPLATE (create the table with the appropriate text and then right click the table to SAVE AS A TEMPLATE.It will get saved in your table files folder and then whenever you require it .You just need to drag and drop it) rather.

I am attaching a video herewith showing the double balloon symbol and how you can edit the master definition.I hope this is what you were looking for.

Best Regards
Kapil Sharma

 

[adam1986]

we would want both single and double circles so would have to create a new entity.
I Will pass this onto the admin guys as i know they are still having a few problems with symbols when we migrated from NX6 to 8.5

As for the doglegged question, attached is a pic of what we currently practise.

We Sketch an offset (usually @45` and 3mm) then sketch another leg, dimension from the centre of this leg to an actual point (or top another leg if required).

We then colour the dimension red to show that it has been manually updated and will require user intervention as it will not associatly update with the model.

There must surely be a better way of doing this, all CAD systems i have used before you simply click the dimenion and it creates a jog for you to repostition from that point?

 

[cowski]

When it is difficult to tell what a dimension is attached to, we will often change the dimension style (Line/Arrow tab) "F" parameter. This will angle the extension lines away from the geometry and often clarifies the intent.

www.nxjournaling.com

 

[JohnRBaker]

Here's an example of something you could try which is a combination of what cowski suggested and using what's called a 'Narrow' dimension:

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.