Autodesk Inventor Sheet Format: Block out your drawing views
Posted on December 11, 2013 by Mark Lancaster, Synergis Manufacturing Product Support Specialist:
The other day I was browsing through my technical drawing (manual drafting) book and came across a section about laying out the views on your drawings. It described how the “draftsperson” should take extra steps in determining the spacing between the (drawing) views that will end up on the drawing. It goes on to state, you can either “block out your views” by lightly laying them out them out in pencil or cut out/arrange rectangular pieces of paper that closely represent the size of your drawing views. Imagine if we still had to do that today in CAD……
As I continued reading this section, I started to think about the “Sheet Formats” function under the “Drawing Resources” of an Inventor drawing. In theory that’s what this function is doing! I am simply blocking out my drawing views for future use.
The “Sheet Formats” function allows the user to define his/her drawing layout and then by inserting it into a new drawing sheet, the drawing is automatically created for you. Okay, maybe not 100% but it is still a time saver, especially if the drawing layout is always the same.
If you start an Inventor drawing using one of the provided templates (I’m using the Standard .IDW). Expand the Drawing Resources/Sheet Formats in the browser window and you will notice there are definitions listed there.
For example, if I “right mouse click” on the definition of “D size, 6 view” and select “New Sheet”, Inventor will prompt for the model to use.
Once I select my model, Inventor is going to automatically create a new sheet representing a “D” size format and define the 6 drawing views of my selected component.
However, these definitions are not restricted to just creating views on your drawing. Certain annotations like view labels, notes, general tables, and sketched symbols can also be included in these definitions. You could also define a definition just using those types of annotations if you wanted to.
For example, let’s say for every machined part I designed for my company, I have to create a “C-size” fabrication print that contains the necessary views, a tolerance table, and some fabrication notes. However before making any changes to your template, I would recommend creating a backup of it.
Now I need to open my Inventor drawing template and start laying out my drawing views using a widget. This widget is only a guide in defining the view layout you need and does not need to represent anything you currently design and/or build. However, if you are going to use model iProperties in these “sheet format” definitions, then it must also contain the same type of information.
In my example, the template I am editing is already set to a “C-size” format, so I am going to start out by creating a 2nd sheet in my template drawing. By creating this additional sheet it will make it easier for me to cleanup my template at the end prior to saving it.
Now I am going to arrange my views as shown on drawing sheet 2.
Followed by defining what my views would look like (i.e. view scale, hidden line removal, view labels, and etc.).
Avoid defining view labels in your layout on any view that is projected as the label will reset to the default settings when the definition is placed into your drawing.
Next I am going to define my tolerance table and fabrication notes on my drawing.
In my example, I am going to add the “material” iProperties of my model along with the “description” property (for blank size) in my fabrication note. Outside of the note definition, I am going to include a few sketched symbols (surface finish and weld symbols) to complete my requirements.
Prior to completing the “sheet format” definition, I would recommend for you to review your layout to ensure everything is correct prior to saving it. To save your definition, simply right mouse click on the active sheet in the Inventor drawing browser window and select “Create Sheet Format”.
Next define the definition’s name and select the OK button to continue. My definition now appears under the Drawing Resources/Sheet Formats section of my template.
Now let’s give this definition a test run and see if everything worked properly. Right mouse click on the definition, select “New Sheet” and tell Inventor which model to use. Here is the result from the component I selected.
If everything worked out properly in your test, the next step would be cleaning up the template so it can be saved for future use. Since I created my definitions on sheet 2 in my example and tested it by creating another sheet, I can now simply delete these additional sheets prior to me saving the template. Once saved, close out the template and now I can start using this definition in future fabrication prints.
I hope that helps you stay ahead.
Mark Lancaster is the newest member to our Synergis technical team, having just joined us back in August. His most previous experience is as the CAD Design Manager of Pall Corporation, one of our long time customers. In that position, he was responsible for workstation optimization and design management, established uniform standards for the local and global offices, and developed global systems to control and manage their design data.
Have a question for Mark or any of our technical staff? Contact us and we will get back to you quickly.