Symbol in a table cell

[Dale_Rosema]

Is it possible to put a symbol in a table cell?

In this discussion there is a .pdf about making templates:

http://communities.ptc.com/message/209849#209849

On Page 46 it shows putting a symbol in the drawing template. Is it just being laid on top of the table or is it actually part of the table that can be saved out and brought into other drawings?

Thanks, Dale

[TomD.inPDX]

It is just placed on the drawing.

[James62]

Yup, it's possible:

http://communities.ptc.com/message/186376#186376

You can use a table to load symbols into your drawing in case you haven't got them in symbol gallery.

[TomD.inPDX]

Nice Jakub. I totally missed that at the time:

I do have a little bit of transportability of using the symbol in this way. It has the entire path -locked- into the note. Once the symbol is added to the part/dwg/format... whatever, it is part of the file. Any way to just use the symbol name without the path? Any problem sharing the file?

[James62]

It would require some testing, but I might not be wrong while just guessing now, that the table when being created, and when symbols are being added to it for the first time, requires all the full paths to be stated. That should be applied if the symbols are not in the symbol gallery of the drawing to which tables's the symbols are being added.

Let's just better put it this way:

1. If you already have the required symbols in the symbol gallery of the drawing where you create a table or a note with these symbols then the syntax could work like this: &sym(SYMBOL_NAME)
2. If you don't then you should state the full path for a note, and have the symbol file (*.sym) on that stated path. Once the symbol is loaded into symbol gallery, which is what the full path does, then you can move the symbol on your disk elsewhere, and the drawing will remember that symbol. Or open that drawing on someone else's comp.
3. With tables it's a little different, because the table when created, and saved into *.tbl file, remembers the symbols that have been inserted in there. So even when it also remembers the full paths which it was created with, these paths to symbols are no longer relevant for that table. This table from *.tbl file will always bring all the symbols it carries into the drawing's symbol gallery.

Anyway, Tom, I think you shouldn't really be worried about these things, and just simply use full paths everytime, which is what you can have saved in a text note, that you can then load into a drawing easily with a mapkey. You can even have a mapkey to type in the whole thing for you.

I'll send you that table via email.

[TomD.inPDX]

That worked! Thanks Jakub. I sent you a reply if you wish to expand on the thought.

[Dale_Rosema]

Jakub,

Thanks. I really appreciate all the help that is available through this forum and for the occational laugh. Dale

[James62]

You're welcome. Just realized the reply I wrote above isn't absolutely right, because according to the picture up above the note doesn't load symbols into drawing automatically even whenfull paths are stated.

Well, I guess that's not what you asked for in the first place anyway.

What bugs me a lil is that I can't edit my own post here now, so it's like written into a stone. Just like all of my mumbling around these boards.

[Dale_Rosema]

It worked yesterday, but that must have been since the symbol was loaded into memory. Today, it is not working.

What were you going to say about the not loading the symbols?

[TomD.inPDX]

What if you loaded the symbol in the part/asm file used in the drawing?

[Dale_Rosema]

The symbol in my case is the company logo. Not really needed in the part/asm file. I was just using that case as an example.

[James62]

Ok, try to follow this:

1. Open up a drawing with table that has an empty cell for you logo.
2. Right click on the table cell, and choose Properties, then in the properties window put in the symbol syntax with full path e.g. &sym(C:\ptc_stuff\pro_e_stuff\symbols\company_logo). When you confirm the properties box the logo should show up. If not then try to load the symbol into drawing's symbol gallery first.
3. Just in case, make sure you got the syntax right, and no spaces in the path.
4. Next, save the table into *.tbl file using "Save table as file" or so.
5. Then load this *.tbl file into your format, or any drawing. The logo symbol should show up.

If this doesn't work then pm me your email adress. I've sent just my table with symbols to Tom, and all the symbols showed up for him once he loaded the table into drawing. He's sent me the picture of it back.

[Dale_Rosema]

Where do you find the path for a drawing loaded into the system. I am trying to verify that I don't have multiple files where it is trying to pull the symbol. I think I get it set with formated and saving out the table. The I try again and just get the &sym(networkdrive:\pathname\directory\complany_logo) show up in the cell.

[TomD.inPDX]

Jakub Fojtik wrote:

<snip>

1. Right click on the table cell, and choose Properties, then in the properties window put in the symbol syntax with full path e.g. &sym(C:\ptc_stuff\pro_e_stuff\symbols\company_logo). When <snip>

Interesting thing I found yesterday in making a new format. I wanted to put a surface finish symbol in the table.

I put... SURFACE FINISH &sym(full path - file name - no ext) and it failed to even look for it.

I then went back and added the brackets and style delimiter:

SURFACE FINISH {0:&sym(full path - file name - no ext)}

...it worked beautifully.

I do get prompted for the value of the variable I added in the symbol. It doesn't know to look for it in the part relations.

[James62]

Right, I suggested that {0:& } thing to Dale in a pm.

If you've got the symbol in a table cell, and you want it to be filled in automatically based on a part relation then I guess it would be best to build the table such that the associative text is inserted there as a note, and not as part of the symbol.

It might be a mess but you will only have to make it one time, cause this whole table can be put into a format, and then you know how the rest of the story goes.

First make a dumb symbol with an empty space in it. In the table make a cell that looks like just one cell, but is made of at least two cells, and erase the inner table border lines. Then insert the said dumb symbol in one of these cells, and the associative note such as &NOTE to a cell next to the first one. After that adjust the dims of whole thing (table cell widths, symbol size, note size, etc.) so it looks like it was always meant to be together. Now you are done.

Let me know if this doesn't make any sense, I can be alot more descriptive.

[TomD.inPDX]

Jakub Fojtik wrote:

Right, I suggested that {0:& } thing to Dale in a pm.

...

What's wrong with that picture, Jakub

Your suggestion makes sense but is quite ugly indeed. There is some kind of propogate option in the symbol but I don't know how to use those. The value is easy enough to change by clicking the symbol and editing the value.

I was working on a drawing I did in Cadkey back in 2007. It is utterly amazing what Cadkey could do that Creo just won't.

[James62]

Picture? I'm just joking there. Unintentionally of course.

Yeah, the solution seems ugly, but should work pretty well.

A symbol with predefined variables can be modified just by double clicking, which sounds good, but you can do the same with user-defined parametric notes.

Try defining a NOTE parameter in the part, and then putting just &NOTE in a drawing table cell. If you define it in this simple way then you should be able to redefine that model parameter directly from the drawing table just by double clicking on the note text in the table cell. The model parameter should then contain whatever you need.

I thought you talked about relations, which should make the note parameter locked, so that way you wouldn't be able to edit it by double clicking from drawing table.

Where do you find this propagate option in symbol definition? I would guess symbols alone should be able to do what you describe.

I've heard Cadkey was pretty timeless back then when it came out, kinda like Rhino. Oh, well, you know too well that Creo comes from Pro/E, and in Pro/E for all problems that may seem simple, there is always an ugly workaround, because in Pro/E there are many things that can't be dealt with simply.

Is it all because the programmers of Pro/E were trying to save few bytes of code? I don't know. Is Pro/E a monster? I'd say, yeah.

[TomD.inPDX]

Right, I drive the formats from Relations in the active part. So you cannot edit those (intentionally...) I added dwg_sfra (which is \dwg_sfra\ in the symbol) in my part relations but this is ignored. The symbol is in the format as a note (as discussed above).

The propagate shows up in parameters when editing symbols...

This is what got me...

What is the name of this kind of tangency display?

This was available in Cadkey and in Unigraphics NX. Seems a lost art. Do we have the option in Creo and I just missed it?

[James62]

Ahh, nice find there. Tom.

From Creo Help:

To Redefine a Symbol

1.
Click Format ▶ Symbol Gallery. The DEFINITION menu appears.
 

2.
Click Redefine. The GET SYMBOL menu appears. Use the Diagram Item or 
Symbol filters to select the required symbol.
 

3.
Select an instance of the symbol to edit or click Name to select a predefined symbol 
from the Select Symbol Definitions dialog box and click OK. The symbol is placed in 
the drawing.
 

4.
Use the SYMBOL EDIT menu to make the edits. 
If you edit the drawn symbol, all instances are updated. If you edit symbol parameters, 
you can check the Propagate option to globally update the symbol instances in the design. 
 

5.
Click Done/Return, when you finish.

If I understand it correctly, ticking the propagate option makes the symbol variable to show the same value in all other symbols of the same name, that are in the drawing. Whenever you change the variable in one instance of the symbol, this variable will also change in other occurences of the symbol in the same drawing.

There is a option to do nice documentation in other Creo module. It used to be called Arbortext. I just can't remember what Creo name it has now. It has an option to make good looking drawings that are associative to original parametric models.

[Dale_Rosema]

Something missing:

I added the {0:& } thing, but I find that if I preload the symbol in the drawing, it loads into the table but if it not preloaded it will not come in correctly.

Any more thoughts?

[James62]

Ok, forget what was said above, and follow this:

1) Make a symbol.

2) Save it as a symbol file, and remember the full path where it is saved.

3) Scrap the drawing where you've made the symbol, and start a new drawing.

4) Make a table, and put in full path to your symbol with the &sym syntax as in previous posts. The symbols should load, if not then load the symbol into the drawing symbol gallery first.

5) Once the table shows the symbol, save it as a table file.

6) Scrap this second drawing as well.

7) Move the symbol away from the folder where you've placed it in the 2nd step.

😎 Start a new drawing again

7) Load in the table.

The {0:& } thingy is still required. If this doesn't work then pm me your email adress, and I'll see what I can do.

[Dale_Rosema]

This is one of my old threads, but just curious. If for some reason the path to the symbol is not in the config.pro, could that be causing it to not load automatically without it being there first?

I have a mapkey that will load the symbol. If I load the symbol but don't "place" it on the drawing but exit out. The when I bring in the table with the {0:& }, it will place the symbol correctly.

Getting closer, but still not sure why this doesn't work.

Thanks, Dale

[cspinelli]

hello James,

i have a question: is it possible to add a relation in the model like this:

IF PARAMETER==YES

PARAMETER_2 = &sym(symbol)

ENDIF

thanks

[BrentDrysdale]

Hi Dale,

Don't use Tables that much but we do use a method to add symbols to dimensions by adding an aligned note to the dimension and this works well even if it is a kludge.

But the thing that allows it to work is sort of hidden and relates to our drawing templates. When I made these latest ones I called up a format as usual but I added the new symbols we wanted to use off the edge of the drawing template then deleted them and saved the template. This saves the symbols locally inside the template and means no path is required for them. Now if a user wants to use those symbols they are in the symbol palette and they can be called in when text editing a note. I think it is this last functionality that you will want.

Hope this helps.

Regards, Brent