"strike thru" text

[Dave K]

NX6.0.1.5 MP1

Is it possible to "strike thru" text? text in a table, to be specific. Since the "table" is like an MS Office spreadsheet, I would guess it's possible, I just haven't figured out how, if it is.

Thanks,
Dave

-Dave
Everything should be designed as simple as possible, but not simpler.

 

[JohnRBaker]

Sorry, but there is no support for notes in NX to be shown as a 'strike-thru'. The only thing that one might do would be to created a modified font where every character has a 'strike-thru' line already defined and you would just edit the 'font' of the text which you wished to 'strike-thru' replacing the current font withe new modified font.

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/

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

 

[hudson888]

Dave,

You could just use a line I guess, or create a separate note comprised of line characters using $b. If you use such a note you would simply position it over the text on the drawing that you wish to strike through. to control the length of the line either scale it up or concatenate $b$b$b, and if necessary set the space factor to 0.01 to give the appearance of a continuous line.

Why I really posted if I may is simply to ask why you wanted to do this. I would simply delete or replace and incorrect text with the desired values.

Cheers

Hudson

 

[JohnRBaker]

OK, I created a modified 'blockfont' which I've named 'blockfont_strike-thru' which can be used to create notes with a strike-thru appearance. I've attached the NX font file.

Give it a try and see if it works for you.

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/

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

 

[Dave K]

John: Thanks. I ended up just drawing a line thru it, but I'll give the font a try too.

Hudson: The reason is for a revision, We use a table for our parts list, so I want to "line out" an obsolete part. I suppose I could just delete it (ie leave blank), but this is how I've done it in the past (previous jobs).

-Dave
Everything should be designed as simple as possible, but not simpler.

 

[ewh]

There is an option in Customer Defaults to strike thru deleted parts list rows (if they had been locked).

The Edge... there is no honest way to explain it because the only people who really know where it is are the ones who have gone over. - [small]Hunter S. Thompson[/small]

 

[hudson888]

ewh,

I thought that was it. That's why I asked.

It really is the only place you'd use it and mainly because some people put systems in place that perceive the need to keep the drawing item numbers the same and such other nuisances.

Gunman,

You need to actually create a part list rather than using a tabular note in order for this to work. The part list and a table look similar to some degree but the part list does possess greatly superior functionality for the purpose that it was designed to meet.

If you're struggling with part lists, think that they are deficient to your needs and have elected to force things to work otherwise by using a table then please post back. Let us know you difficulties we'd either be glad to help or keen to learn what challenges you.

Best Regards

Hudson

 

[Dave K]

I just haven't had the time to get into using the part list functionality, and "legacy" data is all done with tabular notes.

One of these days I'll get some spare time to play with parts lists.

-Dave

-Dave
Everything should be designed as simple as possible, but not simpler.

 

[ewh]

It may seem daunting when you first start to use parts lists, but you can quickly get used to their quirks, and the effort is well worth it.

The Edge... there is no honest way to explain it because the only people who really know where it is are the ones who have gone over. - [small]Hunter S. Thompson[/small]

 

[Dave K]

Will it work for files that do not contain components, ie a weldment, where all the pieces are modeled in one file?

-Dave
Everything should be designed as simple as possible, but not simpler.

 

[jerry1423]

No, It will not work unless components are involved.

I am a fanatic about NX, but it would be nice if it could do weldments like SolidWorks can.

 

[hudson888]

Sorry Jerry,

That's not true it can me made to work with files like weldments although I don't create weldment data all in the one file myself. But any assembly even if created as a collection of solids can be used to build a parts list with a moderate amount of extra effort.

To use that technique requires that you assign attributes used in the parts list to the SOLID BODIES not features, and then manually add the solids to the parts list levels. When you get more involved with working with parts lists you'll probably follow that logic a little better. The upside is that you will find the callouts and ID labels better and easier managed for you using those tools. The downside for non assemblies is that you have to force it to work somewhat, and I would really say that I'd break down the models into assemblies where possible.

Now for Weldments My preference is to create assemblies of the cut plates or tube frame elements assigning attributes for the size/length/thickness of the material as I go . If you need to represent them as united or post machined you can either link or promote the bodies in your weldment assembly and unite/drill and tap/machine by modifying those solids. There is conjecture among some users but I greatly prefer promotions for weldments, even though it is the only place that I use promotions, but it seems to me simpler and more straightforward. I use a parts list to work with the bill of materials identify cut lengths of standard section with ID callouts and reduce the number of dimensions required to complete the drafting task.

Good luck with it there's a bit here to absorb in one sitting and I know that I can only really skim over it in a quick posting.

Cheers

Hudson