Drawing label question

[Anonymous]

I started working for a company where a lot of work has been done but the people who did the work are no longer here.  There are drawings they did that I am trying figure out how they did certain things.  One thing is how they made a label for their drawings.  Every drawing they did they would add a label under the isometric view.  It would have be a text label where eveything in it was basically made from model properties (see attached picture for more info).  I can remake this label easily by creating a text note and then editing the format, going to the "type" area and putting in each property.  Then I have to change the font size of the top two (see picture).  Is there a way to make up this label and just insert it everytime? 

Also, the "view label properties" under type doesn't exist.  Does anyone know why this is?

I'm using Autodesk Inventor Professional 2010

[AlisonDavis]

Hi,

It's likely a sketched symbol, under Drawing Resources in the document.   You can create the text with the parameters in the sketched symbol and then insert the sketched symbol into the drawing.  Drawing resources can be shared between documents by using the Drawing Resource Transfer wizard.  Or perhaps your predecessor had the symbol stored in the drawing template.

Regards,

Alison Davis

[Anonymous]

Thanks for the response.  I'm not sure if it is  a sketched symbol because when I open the drawing resources folder there is no plus sign beside the sketched symbols folder.  I've never used sketch symbols so I could be wrong though.  Also, I noticed that I can only delete it if I delete the isometric view.  Therefore Im thinking that he somehow has linked it to the view.  I'm imagining that when he places the view it automatically places this text label with the iproperties already in it.  Is this even possible to do?

Thanks again

[jtylerbc]

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@Anonymous wrote:

I'm imagining that when he places the view it automatically places this text label with the iproperties already in it.  Is this even possible to do?

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Yes, very possible - I was using it myself all morning.

In your Styles and Standards editor (pick your Standard, then the View Preferences tab), you can set up default values (including iProperty references) to appear in your view labels automatically.  I'm just using it to insert the part number where the view name normally is, but of course by inserting more properties you could do much more than that.

 

[Anonymous]

Perfect!...There is one more question though that came up.  Once I have changed the the style how can I save it so it always this way?  I can change the style and it will change for that specific drawing but when I close and start a new drawing everything goes back to the way it was.  I have checked out the project file and changed the status of the style library to write but it's still not saving.

[jtylerbc]

Assuming I'm understanding the question correctly, there is a step you're missing.

The styles exist in two places - a local copy in your document (which is what you changed), and a "master" copy wherever your style library is located.  If your settings tell Inventor to use the Style Library, then whatever is in the library will override the styles in the template when you make a new document from it.

Having the project file set to Read/Write does not actually SAVE the styles to the library, it just gives you access to the command to do so.  From a drawing where you have made the change, click the Manage tab.  On the Styles and Standards panel, click "Save."  After it thinks for a bit, it should come back with a list of styles that are different between your document and the library.  Make sure the appropriate ones are set to "Yes" in the "Save to Library" column, and click OK.

If you are making the modifications and saving the styles from your template, you should be all set.  If you did so from another drawing, you will need to also open up the template and use Update Styles, so that the local styles in the template and the new library styles agree.  Failure to complete this step will result in an annoying warning message every time you start a new drawing, and may cause the overwhelming urge to punch your monitor.

[Anonymous]

Nicccee....thanks again

[jtylerbc]

You're welcome.

Another trick you can use with this (which is what I'm actually doing with it):

If you have different drawing types that would have different labels, you can set up different Standards for each, which otherwise use the same styles (unless you change those as well).

For example, for my individual fabrication details, I want it to put the part number in the label, which was my example from earlier.  However, on the fabrication assembly drawing, I don't want this, since they would all be the same.  So, I have a standard with the automatic part number labels, and another that uses the default Inventor settings.

Before I start placing views, I just go to the Document Settings for the drawing, and activate the standard I need.  I've only been using it for a week or two, but so far it has gone well and saved me a ton of time manually messing with labels and other styles.  I wish I had figured all this out a year ago.