Custom .dwg template

[DaveyL]

Bonjourno,

Brief explanation, I work for a company who has recently purchased Autodesk Inventor 2012, amongst other Autodesk products and I have had some basic training from a local company. My background is Ideas11 at uni but I believe I have got a good grasp of the basics of Inventor. Although I do only have maybe 2 weeks solid hands on experience.

Anyway, the company who gave the training set up a .dwg with our company name, details etc and when it is opened (it is in templates folder) it asks for a few 'Prompted Texts' like description, scale, paper size. After entering these details a warning about a Style conflict comes up. This says Style definitions in template differ from style library, library definitions will be used. It does not seem to affect the document but if anyone can suggest a fix that would be appreciated, it is out of my depth.

However, this is not the main issue. Each of the parts that are placed into a .dwg file has a part number and this has been set in the part properties. There is also a field in the template for part number however it is blank. Is there a way to automatically put in the part number in that field taken from the .iam/.ipt file?

I've searched the forums for a similar post but if there is one (which there probs is) I can not find it. Any help would be greatly appreciated,

Dave

[jtylerbc · Accepted solution]

For your first question:

Styles in Inventor reside in two locations - local copies within the document, and the master in the Styles Library.  The Styles Library is one of the items controlled by the "Design Data" file path in the Inventor Application Options.  The warning message you are getting is telling you that there is some conflict between the two, and that it is choosing the library version to use.  Most likely this is something that has been modified in your template, thus making it different from the definition in the library (which is probably still at the default settings).  If this is the case, you will need to open your template drawing file, and save those differing styles to the library.  This will be done from the Manage tab, Styles and Standards panel.  I'd recommend reading up on the Styles Library in the Help, as well.

For your second question:

In your drawing template, click Tools, then Document Settings.  On the Drawing tab, there is a button "Copy Model iProperty Settings."  Click it, then check the appropriate boxes for the properties you want to copy over when you create a drawing.

[DaveyL]

Thank you for your speedy reply. That has solved the issue but I think I may need to venture into this to gain an understanding of it in the future, unfortunately I appear to be one of the most advanced users in the company.

Dave

[Curtis_Waguespack]

Edit: it looks like you figured it out from the previous reply while I was replying! 

 Hi DaveyL, 

To resolve the situation with the styles conflict:

• Close all Inventor file and then go to the Get Started tab and click the Projects button, and then make sure the Use Style Library setting is set to Yes
• Then open the template file by browsing for the template with the Open button  (rather than the New button, which creates a new file based off of the template).
• Then go to the Manage tab and click the Save (or Save Styles to Styles Library) button found on the Style and Standards panel.
• Then you can choose the styles that you updated in the template file and push them to the Styles Library file (an XML file that Inventor uses to manage styles)

As for getting the title block to read the model's part number property, you'll most likely want to edit the title block definition and redirect the Part Number text field to have it look at the model properties all of the time.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[jtylerbc]

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@Anonymous wrote:

Thank you for your speedy reply. That has solved the issue but I think I may need to venture into this to gain an understanding of it in the future, unfortunately I appear to be one of the most advanced users in the company.

Dave

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I understand that - I had the same situation when I first started with Inventor at my previous employer.  I was officially in charge of administering and training others on the system before I even had the training myself!  Fortunately the help is usually pretty good, and there are a lot of online resources.  Unfortunately, I didn't find these boards until after I had already stumbled through a lot of things on my own - could have saved me a lot of trouble.