iProperties Issue

[Anonymous]

Hello, I recently designed parts, put them in an assembly, and then used the presentation to separate all the parts from the assembly and placed that into a drawing. Now that I have everything marked up I want to make another sheet and start to dimension each individual part. However, after dimensioning a part I can't make the title block different from the first sheet. I can't find iProperties for the individual part to change the title block. Is there a way to change the title block without doing it manually? The whole time I've been using Inventor I've just been making separate drawings and using iProperties to change the title block, but then it says sheet one of one even though there are multiple papers I'm printing out.

[Cadmanto]

The properties carry through the drawing with multiple sheets.  If you want the properties to display different values for each part, then you are going to have to create separate drawings.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[mcgyvr]

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@Anonymous wrote:

Hello, I recently designed parts, put them in an assembly, and then used the presentation to separate all the parts from the assembly and placed that into a drawing. Now that I have everything marked up I want to make another sheet and start to dimension each individual part. However, after dimensioning a part I can't make the title block different from the first sheet. I can't find iProperties for the individual part to change the title block. Is there a way to change the title block without doing it manually? The whole time I've been using Inventor I've just been making separate drawings and using iProperties to change the title block, but then it says sheet one of one even though there are multiple papers I'm printing out.

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What specifically do you mean by "used the presentation to separate all the parts from the assembly" ?

And what specific "file" are you using to place each base view?

Its entirely possible to have a complete assembly shown on sheet 1 and the title is pulled from the iproperty (description or whatever) of that specific assembly and then to place a base view on sheet 2 (using that ipt file as the file) and the title block will show the iproperty (description) from that specific part file and not the assembly..

So its entirely possible to have a different title block for each sheet... That all depends on what field your title blocks are referencing and from which file is being used as the base view (or more specifically the first placed view) on that sheet

[japike · Accepted solution]

If you set up your title block to look at model properties then the first model you place on a sheet should determine where the properties come from. You could set up a title block to grab drawing iproperties for the general stuff. Then set up an additional title block with the description set to model properties, for example. Use the second title block on additional sheets of your drawing and they should get their description from whatever part is placed first. Hope that makes sense.

[CAD-One]

While in inventor drawing (idw), right click on the file icon & select "new sheet".

The total # sheets automatically updates. See the image

http://help.autodesk.com.s3.amazonaws.com/sfdcarticles/img/0EM30000000V54Q

Hope this answers.

[mcgyvr]

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@Anonymous wrote:

but then it says sheet one of one even though there are multiple papers I'm printing out.

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@CAD-One Good catch there on that part of the question.. I didn't read all the way to the bottom.. But I think they know how to add a new sheet their title block just isn't setup properly either..

The answer to this also depends on how your title block is setup.. There is a property of <Sheet Number> and then another for <Number of Sheets> that needs to be in your title block if you want it to say "1 of 2" The 1 comes from the sheet number property and the 2 comes from the number of sheets property and you add a "of" in the middle or whatever you want..

This is how mine is setup.. It doesn't wrap like that when its only 2 or 4 or whatever..

[Anonymous]

When you make a new file you can make a presentation of the assembly and separate it, it's the .ipn file. It's used to show what the assembly looks like when it's taken apart. I'm not sure if that has anything to do with it but I can't have a sheet that has different properties on the title block than the first one. I figured since inventor has "sheet X of X" on the title block, I assumed that it was possible to change the properties without manually editing the title block's definition.

[Anonymous]

Thanks a lot, I edited the title block definition and was able to change it so that it chose the model instead of the drawing.