Varied title block information between each sheet in one .dwg??

[Anonymous]

I am new to Inventor LT 2016.  For assemblies in AutoCAD I would create everything in model space and have a different sheet for each part, each having its own part number, material, etc.  I cannot do assemblies with LT (I rarely have more than 3 parts to an assembly) but I have made multi body parts, create a second sheet with the views and dims copied over and then turn off the visibility for the body not to be represented on that sheet.  My problem is that the title blocks information is the same between ALL sheets.  Its fine that the first sheet's title block info is connected to the Iproperties, but if I change the second sheets title block information the first sheet title block changes as well.

Is there a way around this??  

Thanks,

Zach

[mcgyvr]

The title block is probably set to pull the information from the parts iproperties and is pulled from the part thats used as the "base view"

Since you only have 1 part then the information WILL be the same.

The only way around is to manually enter the information instead of pulling from a parts iproperties.

[Anonymous]

When I go into sheet 2 and manually change the title block information, those changes happen to the title block in sheet 1 as well.

Zach

[mflayler]

You can do 1 of two things...

1.  You can create a new Titleblock for Sheet two that uses Custom iProperties that you would enter in your MB part file.

• PartNumber2, PartNumber3, Description2, Description3
• In the secondary and tertiary TBs you would customize them to read these properties instead of the basic Inventor iProperties

2.  You can use the Make Part or Derive command to save them out as individual files (.ipt) and assign standard information to them that way.  Then when you put the model into Sheet 2 its a different file and has a different set of iProperties than the original.

Here is a paper attached on customizing your template and styles in case you are new to this...

[mcgyvr]

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@Anonymous wrote:

When I go into sheet 2 and manually change the title block information, those changes happen to the title block in sheet 1 as well.

Zach

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post your idw template file so we can see exactly how its setup to prompt or not,etc...

[Anonymous]

Mark_Flyler:  I will read that paper, thank you.  MB = multi body, what does TB stand for?

I derived the orginal .ipt.  I then added another sheet to my original .dwg and put the base view in from my derived part.  My title block on this sheet is still connected to the information in the original .ipt.  I opted for this route thinking I didn't need another title block.  Do I need to create a new title block for the derived part option to get the results I am looking for??

This route also means all new views and annotations.  The vast majority of the dimensions and views will transfer over to both sheets. As an example, picture creating a model of a plastic water bottle along with its cap all in one .ipt.  Sheet one will be the bottle with cap installed and final dims.  Sheet two being the bottle (many of the views and annotations from sheet one will be copied over, but the cap body visibility will be off).  Sheet 3 being the cap.  This is what I am trying to accomplish so that when the drawing is opened it can be done so by the part number of the complete bottle and all parts associated will be in one drawing, just on different sheets with different title and drawing number in the title block.

I attached my .dwg template, but I don't believe mcgyvr is following what I am saying.  No matter what I change in my title block in one .dwg file, every title block will match on each sheet.

Thanks,

Zach

[mflayler · Accepted solution]

Its because your drawing template is reading the iProperties of the drawing file and not the Part file.  You will have to change this to make it work.

You could either make this field a Prompted Entry so that you can change it manually when you create new sheets each time or...

You could change it to read the Part iProperties instead so that it reads the iProperty information of the IPT instead of the DWG.

I would sooner do the latter as I would want complete iProperty information in my IPTs.

[mflayler]

TB=TItleblock

[mcgyvr]

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@Anonymous wrote:

I attached my .dwg template, but I don't believe mcgyvr is following what I am saying.  No matter what I change in my title block in one .dwg file, every title block will match on each sheet.

Thanks,

Zach

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I follow you exactly.. 

The template file I requested shows the exact problem clear as day.. Which mark already pointed out in post 7 so I don't need to cover it again...

Your drawing is behaving exactly how it should given the way it was setup.. Thats why I requested it.. Because its now 100% clear and didn't require us asking numerous (or any) additional questions..

[Anonymous]

OK, so when using the derived method, changing the title block iproperties link from properties-drawing to properties-model fixes my issue with the information being the same on all title blocks, I get that now.  This method requres me to completely build my views and annotations all over again though, which is more work that just changing a few items in the title block.  

What I was trying to portray earlier was that I would leave sheet one's title block linked to the model or drawing properties and then merely delete that link in sheets 2 and 3 and then write in what I wanted manually for those two title blocks.  When doing this EVERY title block would change.  If this would work it would be the fastest route for me.  Please confirm, but I am guessing to do this I would need to insert a different title block into each sheet.  In the end, I'm not sure this will be any faster than using the derived part method.  My big concern with derived part is editing the final assembly, will the derived part update as well??  I will have to use this method a few times and see how it works for me in the end.

Thanks for the continued help guys,

Zach

[mflayler]

What I wanted to do was set you up for future work to operate this way.

Regarding your questions...

Derived: Yes, when a change is made to the MB part file, the derived part will update.

Changing out the View in Sheet 2, 3, etc.  You could try the Replace Model Reference command on the Manage tab of the Ribbon in your drawing.  That might let you switch out one of your view placements with your derived part and may keep the majority of your dimensions.  Inventor works pretty well if the geometry is derivative from an original file.

[Anonymous]

I know I'm a little behind on this thread, but I am in need of some help. You say "You could either make this field a Prompted Entry so that you can change it manually when you create new sheets each time". How? I have prompted entries and when I change it on sheet 2 of XX, it changes the title block on all drawings. I am making construction drawings for bolted storage tanks and usually have around 30 different drawings. I need to be able to change the drawing description and number. In the attached PDF I have circled what I am needing to change per "new sheet".

The way I have been doing it so far is to make new .idw for every drawing needed, or transferring everything to AutoCad. Your help would be greatly appreciated.

[SBix26]

In my immediate experience (just now, with Inventor 2019.1.1), using the default English .idw template, I modified the title block to pull model properties instead of drawing properties and added one prompted entry text to it.

It works exactly as you are requesting.  Each new sheet prompts for the new field that I added to the title block, and when a base view is added to the sheet, the model's part # and description are added to the appropriate fields.

What version of Inventor did you say you were using?

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Sam B
Inventor Pro 2019.1.1 | Windows 7 SP1
LinkedIn

[johnsonshiue]

Hi! It depends on how the two fields derive the data from. If they are static prompted text, you should be able to edit the title block and change it. If they derive from the iProperties of the assembly, you will need to change the iProperties or turn it into a new title block and make change to the title block definition.

Based on the PDF, it is unclear to me how the two fields were created.

Many thanks!

[Anonymous]

Thank you. I had to try a few different things, but this worked as I had needed. You're the best!