Create text curve on 3D modeling based on attributes 3

[JBIM]

Hi everybody,

I need to find a way to identify my components directly on the solid body : It should be something like an undercut box with engravement (3D or 2D line)on it.
I need it to automaticly write certain attribute using expresion like <W$=@$PART_NAME>.

Basicly, what i need is a way to write the name and material of each part on the very solid I create:
so everyone how open the file will be able to see the caracteristique of the part.

I don´t know if it possible , for example it woulb be ok if I could write associative text (or any kind of text by the way) on sketch.

Runing nx5
thanks a lot

 

[hudson888]

There will be something that you can do with even grip if you really had to, but it isn't as simple as using <W@TEST> attribute to text substitution. On the other hand I don't think it is necessarily a sketching question either. You can create text in the model of course using Insert>Curve>Text, but there is little scope for automating the process that I'm aware of which would not involve creating some sort of programming tool.

It might help your cause if you describe more about what you want to achieve. Some people would want to model text in relief for castings or plastic molded parts. The other possibility is that it could be machined in. And you would want to flag that with the machining guys because there are various tools for doing that, some within NX but sometimes there are other options depending on what your controller supports and what you want to do.

Lastly you could just knock out a parts list to excel and plug that into some form or mail merge to print out sticky labels and identify you parts using that method. I don;t remotely think that's what you wanted but most people don't know that you could do it so you never know.

Best Regards and Good Luck

Hudson

 

[JBIM]

Thanks Hudson888,

Utlimatly, what i need to do is create machined text in every solid body of my assembly with "my" numeration part on it. but it sould automaticly write the text from the part attributes that I previously create.

Just for better understanding :I work in mold making

thanks

 

[mmauldin]

You can add text tot he model by turning off the drawing sheet while in drafting. It's under View>Display Sheet. Once the sheet is toggled off, you will see the model but you will still have all of the annotation commands available. You can now add text to the drawing by using the standard text creation feature to create text that is linked to the attribute. The text will be put on the the X-Y plane of the WCS, so you will have to put the WCS where you want the text. One thing to remember is that the text will not be associated to the model in respect to its position, if the model changes the text does not move with it.

 

[hudson888]

Michael,

While that is a good start, your output is still a note in model space. What is required are curves that can be followed to make a cutter path. You could export the text as a CGM using the polylines method to render it back into lines and arcs once imported, but anyone keen enough to use attributes wants a slicker method than that. It occurred earlier but I think you really want to look at creating a little programming tool to assist with this. I'd wager others out there have something that would at least go close to doing what you'll want.

Cheers Again

Hudson

 

[mmauldin]

Actually, you can use the text directly in UG CAM. You can create engraving on a flat surface using Planar Text Mill or project the text onto a curved surface using Profile Text Mill (I think that is the method, I don't have access to CAM at this moment). This way, the milling function is fully associated to the text, and will update when the text is updated. Breaking the text down to individual lines can cause problems by changing the number of entities involved.

 

[hudson888]

Well done Michael, Shows how long I've been out of the machining game. Looks like we might be in luck with a simpler solution that I thought.

I suppose all that remains is for JBIM to give it a try and hopefully let us know if it suits his needs.

Cheers

Hudson

 

[JBIM]

Hi,

I was reading the post and i have some doubts abouts UG CAM.
Is that part of the "manufacturing module"?
Cause I don´t have manufacturing license

However I think you understand the ideia( It should be easy to create: like running a program or some, and obviously associative)

thanks again guys

 

[mmauldin]

Still haven't been able to access the CAM license, but I seem to remember now that the 3D text milling is under Contour Milling, not Profile milling.

 

[hudson888]

Yes you would need elements of the manufacturing module. If I'm guessing that you use an external toolmaker then send him some data and hopefully he'll make his own arrangements as to how the text is actually machine in.

Regards

Hudson

 

[JBIM]

hi,

Well i still don´t know how i´m gonna do this
anyway I think that we should be able to create text on sketch for that matter:
if it is nedeed to create some text at a certain distance form an edge, right now it is impossible to constrain it so that if you change the edge, the text go along with it.

I think that nx sould look into that kind of need from customers don´t you ?

thanks

 

[hegdedin]

Hi,

I faced the same problem when creating some Mold Wizard Library components.

I created all the text on the surface first and then extrude subtracted them. And then I used 'suppress by expression...' to control all these extrusions one by one.

May be this procedure helps but I had very few configurations.

dinni

 

[hudson888]

JBIM,

If you either go to the trouble of rendering the text into lines and arcs, where we started out on the topic, or develop a program to do so for you, then you may add those curves to a sketch and use positioning dimensions in the sketch to keep it aligned with the face.

If they remain curves then it should be less trouble to manually move them that it might be to set up all the required associativity. If however you use the curves to create features that you boolean with your solid model then you have your answer as to how to not have the model fall over if you make changes.

The general tenor of upcoming changes for NX-6 seems to be headed in a direction that allows you to use more powerful tools to perform changes along the lines of what is currently available in direct modeling, so this very structured approach to change management probably won't be as valuable an investment in your time and effort as to warrant the level of concern that it may currently attract.

Best Regards

Hudson

 

[PHayden]

From drafting, Insert/Curve/Text will create splines of text that can be cut from the model (mileage may vary)

 

[hudson888]

PHayden,

I did canvass that option earlier but you can't give it an attribute, unless of course you create a program to do so.

Nice gear by the way, good to see somebody reads .

Cheers

Hudson

 

[NXMold]

I often use Insert-Curve-Text, and have wondered about this same issue. It seems that we need to get the developers to add the text string as a parameter. That would allow editing text outside the feature dialog, and integration with attributes.

I would also like to see the text command availible inside a sketch, to permit positioning (especially multi-line text blocks).

 

[JohnRBaker]

This is on our list of potential projects for NX 7. NX 7 also includes some major work in the area of attributes in general and so at this point in time, it was felt that we should get the foundation (attributes) fixed before we start putting more bricks on it (additional functions with links to attributes, which will all have to be reworked anyway).

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

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