drawing borders 2

[vitulaaak]

Hello,

I am using NX 3 and have the following question:

lets say we have some borders, that we import when we start the drawings, is it somehow possible to have them with automaticaly filled notes using the parameters? If yes, how can you do that? This is something, what I used in Proe, but dont really know, if it works in UG also.
thanks
Vit

 

[JohnRBaker]

You can create notes in your border that are linked to attributes and if those attributes have been assigned values, when the border is add, they will automatically update to reflect the 'values' of the attributes.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA

http://www.siemens.com/ugs

http://www.plmworld.org/museum/

 

[vitulaaak]

well, i thought it should work, but problem is, that our company borders are imported as a part and therefore i wasnt able to find a way to put the note there...do you have some example?
thanks
vit

 

[vitulaaak]

the thing is, that I cant find an option to change the pattern... I can only replace it or load it...

 

[JohnRBaker]

That's why I no longer use patterns but instead custom symbols.


John R. Baker, P.E.
Product 'Evangelist'
UGS NX Product Line
SIEMENS PLM Software
Cypress, CA

http://www.siemens.com/ugs

http://www.plmworld.org/museum/

 

[vitulaaak]

The custom symbol wont really help...
my expectations were, that in my start part, i define the parameters (drawn, date, part name etc.) and when i start the drawing, they will autmaticaly fill in in the imported borders with the notes....

 

[ewh]

We use seed files for this, which include the pattern and any text we want to be automatically updated with attributes.

 

[vitulaaak]

can you give me an example of such file???
thanks vit

 

[hudson888]

Do you know how to create an annotation that references an attribute in the file. If not it is provided for in the attributes dialog and shouldn't be hard to find. I'll have to leave you to chase it up via the documentation as I can't stay online.

We use templates with patterns for the borders but not the text fields. UG actually is shipped with examples for this that you should be able to find and adapt to your purpose. Very easy and convenient to use.

Regards

Hudson

 

[hudson888]

P.S. add a parts list to your template for best effect. Doing so gives you the ability to automate the display of information from another part, which we use even if it is a detail drawing. Some site like to create separate templates for detail drawings and assembly drawings because they set up the part list levels differently.

Regards

Hudson

 

[vitulaaak]

well,
there are few other questions:
i would like to create a start part with predefined parameters, that i fill in when i start to model the part...
when i do file/properties/attributes i can only define string valued attributes...why? how can I use part weight as attribute?

lets assume that i have all these attributes defines, i have to get them to the borders and here...i dont know how to do that....

 

[ugsoft]

vitulaaak ,

You might be interested in the solution provided on the web:

http://www.ugsoftstore.com/drawing_template_manager.asp

Regards ,

UgSoft

 

[hudson888]

I am writing this as I had done earlier assuming that you're using master model system whereby the drawing and geometry are always in two seperate files.

To edit a parts list what you want to do is select the column and then under your right mouse button select style. If you have trouble with this to start with make sure that you're on object selection mode. In drafting the other common mode is component selection and I keep the icons displayed to deal with getting caught out after changing between parts (see below).

Under the columns tab you'll find everything you should need, column type, key fields and the various available attributes under the arrow icon if you don't want to type in the name.

To gather the mass of loaded parts the attribute is below.

<W$=@$MASS>

under the metric system if you want to use grams as of NX-3 the attribute will be multiplied by 1000.

<W$=@$MASS>*1000

To add attributes to your part files obviously you need a consistent naming standard for the attributes that concurs with the parts list you'll set up.

First off I find it easiest to select the work part from the ANT under the right button select properties and then the attributes tab. You'll see your title and values fields which you fill out and hit enter to accept. They can just as easily be deleted to it's dead easy.

After that I often find a part with the attributes already assigned selecting it the same way off the ANT. From there you can <shift> select a range of attributes, find the copy icon and use it to save those values onto the clipboard. Next you just switch parts to your new model and getting back into the properties dialog use the paste icon to transfer all the values from the other part. A handy tip because often not all the values change and you'll want to keep the same titled attributes for you parts list to work.

Best of Luck

Hudson

 

[vitulaaak]

Ok, this is good but...
the problem is, that it only works in the components table...but i want to put notes on the places i like so that they can call the attributes...thats one thing and the other is, that i still have no clue how to put the notes directly to the borders...

 

[vitulaaak]

ok, i have managed to have the borders with the parameters...the last thing, that i am struggling with is, can i have there the parameters of components??? even though i made the component table in my borders, its not displayed in the drawing, when i bring the borders...(

 

[vitulaaak]

ok, another thing...i made a table of components in my drawing and i tried to put the mass in one column, but it doesnt show anything....

 

[hudson888]

There is another way to get the mass onto the face of the drawing. From the drawing file as your work part and starting in the modeling application you could use expressions to create a body measurement variable of the mass. It will be stored as a parameter.

i.e. p18 in the example below, where you add this note to the face of the drawing.
TOTAL MASS = <X0.2@p18> kg

If you do so in a template and re-use that in a number of drawings then you'll may have to edit the note if the value of the parameter changes because to need to re-create the body mass expression. It is a bit more manual and involved than the simple parts list but it does add up the total mass.

Beware you need to open the assembly fully to get this to work and if a component is not found or deleted in the assembly the drawing may hang upon opening and cause you some trouble.

I think this method quite clever and have seen it used to good effect, but I would steer away from it for very large assemblies.

Now for your other questions. We use patterns that is one file with the basic framework of the drawing in it. The template is a file with the border added as a pattern plus some attributes for items like the date, title, drawn by and perhaps a parts list added. Sounds like you were in part familiar with this.

So to add a title create in the file properties an attribute called title and give it some text in the values field. Next open the annotation editor, and expand the full dialog by clicking on an icon A with the pencil along side. Midway inside that window you should see some tabs and select relationships from the bottom right of the bunch. There are three icons for possibilities including expressions, object attributes and part attributes, you want to use the last one.
If you're hopefully working in a clean part when a list box pops up there will only be one option "title". Move your cursor over the main window to position the text on the drawing. Now you'll notice that what appears is just the text that you typed in the value field. Change the text style, to whatever size and font you like and move it's origin over the appropriate empty spot on your title block of the drawing and you're done.

If you're creating a template then chances are you'll only have to do this once.

Now if you want to pick up attributes from other files you can add text from an "object attribute" by selecting the component and picking one of it's attributes from the list box in the above described annotation dialog.

Better in most cases to use a parts list because it caters for changing components. Using the method above if you were to try substituting the component with the object attribute the note goes stale and needs basically to be re-created to update. It doesn't matter if the component you substitute with has an equivalent attribute or not, the system doesn't buy the swap. Using this method in a template is also unsound.

Hope you get it to work for you. If you struggle or are using a different version than NX-3 then try to pick up on the terminology that I'm using and delve into the documentation I'm sure you'll find what you're missing.

Regards

Hudson

 

[hudson888]

You need advanced assemblies. The mass comes from weight management under the part properties dialog.

Regards

Hudson

 

[vitulaaak]

I dont understand what you mean by this:
There is another way to get the mass onto the face of the drawing. From the drawing file as your work part and starting in the modeling application you could use expressions to create a body measurement variable of the mass. It will be stored as a parameter.

i.e. p18 in the example below, where you add this note to the face of the drawing.
TOTAL MASS = <X0.2@p18> kg

If you do so in a template and re-use that in a number of drawings then you'll may have to edit the note if the value of the parameter changes because to need to re-create the body mass expression. It is a bit more manual and involved than the simple parts list but it does add up the total mass.

the problem is, that i dont understand, if UG already has some parameters ( mass, name etc.) or not... and if yes, why it doesnt work, if i call the mass in the components table?

 

[vitulaaak]

Ok, next thing...when i create a parts list in the drawing, it has no problem, when there are no parts..the rows siply disappear...the thing is, when i create it in the borders, the table wont appear at all...even if the part has components...