total_sheets

[Gucio]

Hi folks,

in drawing there is parameter &total_sheets. This parameters count number of sheets in drawing. It works ok, but what should be done when last sheet contains only external boundries of sheetmetal parts, and this sheet should not be counted. In other word: how to cheat total_sheet parameter??

Sample:

Bended sheetmetal part is shown on first sheet. On the second sheet unbended part is displayed with necessary dimensions. Last sheet is prepared for manufacturing department so part is in 1:1 scale and without any dimension (last page will be exported as dxf). So in general from customer point of view drawing contain only 2 sheets, but total_sheet = 3.

Do you have any idea how to solve it??

thx in advance for any suggesition.

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[DARYLREECE]

Calculate your own drawing parameter as a relation. &my_sheets=&total_sheets-1.

I haven't tested it, but it should work.

If you do this on every type of part, bury the relation in the template for those types.

[Gucio]

thx for your respond,

but in fact it does not work. as far as I know, there is no possibility to use total_sheets in relation.

Total_sheets is hidden and could not be used in "normal" way.

[neomechanikos]

Unfortunately there is no such thing as a drawing relation. The only ways to solve this that I know of (as of Creo 2.0) are the following:

• Create a manually driven drawing parameter that represents the total number of sheets and use that in the format. You will have to remember to increment it manually if you add/remove a sheet but at least you won't have to do it on every sheet.
• Instead of creating a new sheet for an flattened pattern, use the same sheet but move it off of the format plot area. Sheet count will be correct but you will have to manually plot each flattened state "sheet".
• Use two drawings. One for the actual part count and another for the flattened states. The sheets will have to be organized after they are printed or in a separate program (i.e. PDF) if using an electronic copy.

Companies I've worked at in the past use the first method.

[Gucio]

Thx Eric,

your suggestions are clear for me.

• first method can caused problem when user forget to change custom parameter. Be aware that during pesales process, Creo is presented as as fully parametric software. So now asking customers to do something manually -could not be accepted by lazy guys.
• it is ok when u plot drawing manually.
• I've also though about using 2 drawing.

I was also concedering solution when there are to diferent drawing formats: one for smt, other for solid parts. In that way of thinking your first solutions could be used, but instead of adding additional parametr I suggest to put number of sheets as a note (static).

again - thx for your answer.

[KiranJ.]

Simply, put notes on each sheet that

like for customer sheets, 'sheet # of # sheet is for customer use only. for manufacturing use sheet #' and vice versa. It gives clear instructions to the user.

[Gucio]

"Simply" - it means manually??. there is no way to ask customer to count sheets, and force him to write it in note. Why there is no possibility to write simply relation in drawing: "my_total_sheets=total_sheets:D - 1" ??

[dschenken]

He was referring to work that you do:

On sheet 1: SHEET 1 OF 3 IS FOR CUSTOMER USE

On sheet 2: SHEET 2 OF 3 IS FOR CUSTOMER USE

On sheet 3: SHEET 3 OF 3 IS FOR MANUFACTURING USE

is how it could appear, with the text being supplied by use of the correct format for the sheet.

As you said in your first post - you want to cheat. Cheating is not something that should be easy to do.

[Gucio]

So please cross out 'cheat', and instead of it answer a question: is there any 'smart' way to show parameter in drawing that will be calculate in a following way: my_total_sheets=total_sheets:d -1;?

In a sample, when the third sheet contains information for manufacturing, guy that will have to sign a paper documentation for sure will say:'you give me only 2 sheets, where is the last one?'. Last page is not printable.

[dschenken]

No. It isn't smart to show that.

The result you are looking for can be obtained by paying PTC for a custom solution. Your sales rep should be delighted to help.

[Gucio]

David,

I don't know if you have access to ptc.com/support - but if yes, please look at Case Details - 11764712.

I work in VAR company, and unfortunatelly I was asked by customer to find sollution for this issue, and because I don't know how to achieve it -I opened this topic.

thx for your help

[neomechanikos]

Again, I think the answer is no. Without drawing relations, there's no way to control this. You also cannot access the total sheets external to the drawing. In a situation where you have two completely different audiences with two different sets of information, it's begging for two different drawings. I don't think that a drawing relation gets you to where the ideal answer should be. I think you need something more like a "drawing simplified rep" where you can define a configuration for the intended audience but still share information between the representations so you don't have to create duplicate views, dimensions, etc.

There are two more possibilities I can think of, but I've never tried them:

1. Drawing representations. Has anyone dealt with drawing representations? I don't have the time right now to test it out, but if you can turn sheets "on" or "off" then it could be useful in a case like this. A quick scan through the help files didn't turn up any sheet based commands. I might test this out later when I have more time.
2. Drawing program. You may be able to control variables in a drawing using program but I've never done it. I think it's only used to control states, and with that maybe you can turn sheets on and off.

Am I correct in assuming that the manufacturer still needs sheets 1 & 2?

[Gucio]

You reminded me, that some time ago I created drawing that behaved depending on the part on drw. For sure it was done for family table instances (flat state is also an instance). I'm not sure if i used drawing reps or drawing program or both.

Maybe this is way that should I follow by...

I'll check it.

but thx a lot for your engagement.

Manufacturer doesn't need 1&2 sheets, but it will be perfect to keep all information in one drw file.