A recent support case for a customer prompted me to investigate how you may create an Autodesk Inventor drawing that uses the same editable text notes on each sheet of a drawing set.
Using AutoCAD, you can easily do this by creating your text note(s) in Model space and directing a Paper space viewport at the same location. You can easily copy this viewport to each sheet in your drawing set, or even build it into your template file.
Inside of Autodesk Inventor there is no Model space to speak of.
Note: Unless of course you are using Inventor .DWG format whereupon you get a *version* of Model space but it isn’t the same as that in AutoCAD.
So, here are some solutions that may work for you inside of Autodesk Inventor (both of which were helpfully suggested by my colleague Paul Munford, so Thanks!):
Option 1: Insert a Sketched Symbol from Sketched Symbol Library.
((new for Autodesk Inventor 2016/2017 releases))
Quickly access and share your collection of sketch symbols through a new external Sketch Symbols Library. This library is an Inventor drawing file that, by default, is located in a subfolder of the Design Data location of your project. This new feature offers the following new functions:
A search and filter feature in the Sketch Symbols Library dialog box.
Preview the sketch in a preview pane within the dialog box before placing the sketch.
Browser expansion state remains throughout session when placing sketch symbols.
A Sketch Symbol Library can be created in IDW and DWG formats, allowing insertion of symbols contained within the library file from either format.
Save your sketch symbols to a customized library.
In previous releases of Inventor, you had to include all company standard sketched symbols in your drawing template. If you had a great idea for a new symbol, you had to include it in your template AND copy and paste it into every current drawing.
The new symbol library allows you to insert your sketched symbols from a centralised library file that you have set up for this purpose.
Sketched symbols are available using the following button on the Ribbon bar:
When you initially click this tool, you are presented with the following dialogue:
Which as you can see from the image above is currently empty on my freshly-installed-on-Windows 10 laptop.
After creating downloading AutoCAD geometry (from GrabCAD!) for a sketched symbol and defining it as a sketched symbol inside of a standard Autodesk Inventor .DWG I saved the resultant drawing to the Sketched Symbol Library defined in my Application options as:
Having created a “Library”, when I now run the Insert Sketch Symbol tool I am presented with the option of the symbol library I created:
(Two guesses as to what the symbol might be given the symbol name above)
Question? Does the Sketched symbol library file need to be IDW or DWG?
As you can see from the pair of images below, Autodesk Inventor is happy using either:
So that’s option 1 sorted. Granted, I have copied in some familiar geometry from an online source, but if your drawing notes are identical on each drawing sheet, this gives you a simple option.
For a slightly more complicated option, you can add Prompted Entry or Model/Drawing iProperty-aware text values to the Sketched symbol so that you get a dialogue similar to this when you insert the sketched symbol into Autodesk Inventor:
And the resultant placement looks like this:
Option 2: A Simple Autodesk Inventor Part file and accompanying drawing view.
The second option you can use is to create an extremely simple Autodesk Inventor Part file such as this:
Into which you create a 2D Sketch. Inside of the 2D Sketch you insert your text note and format it using the text height and font you expect in your drawing environment.
It is also worth measuring the size of the notes column or the notes location and using these dimensions to constrain the text note accordingly:
Once you have your text note set up to meet the company/customer requirements you can then create a drawing view in your Autodesk Inventor drawing and reference the Part file containing the notes for this particular project/drawing set:
With the drawing view placed, you can then copy it to each and every Inventor drawing sheet as required.
NOTE: when using this method, you need to make sure the drawing notes view is created AFTER the geometry views have been created otherwise any drawing frame text objects that use Model iProperty values such as part number, or Description will pull these values from the drawing notes part file.
In this post we looked at two ways of creating editable generic drawing notes for Autodesk Inventor drawings. The first method uses the new Sketched Symbol Library feature, the second method uses a simple part file.
If you can think of a third way, then please tweet me @AlexFielder
For more Autodesk Inventor tips and to learn about the new Inventor 2017 features, take a look at our Mechanical Blog Category. If you have any enquiries, please send us a message: