Seeing that creating axonometric views is possible in a 2D drawing view, can someone tell me how to create and save a customized axonometric view in the 3D modeling environment?
Currently the only options are front, back, top, bottom, left, right, isometric and random...
Solved! Go to Solution.
Would "View Representations" be what you are looking for?
See if this link helps you as well.
(2 Corinthians 5:21)
Autodesk Inventor LT is not equipped with view representations or assembly mode features. I did however create a tutorial on how to create an axonometric view in part mode. See the tutorial below.
Didn't know you were using the LT version of Inventor.
Never used this version, so I can't help you there.
You never attached the video FYI.
(2 Corinthians 5:21)
Below is one strategy to create an axonometric view in part mode.
Step 01. It's best to create a new file and save the file as a template. Though you can also perform these steps in an already existing part file the benifit of a template is these features will have allready been created and hidden.
Step 02. Make the Y/vertical reference axis visible, or create a vertical axis using the vertical work planes.
Step 03. Create an angle to reference plane.
Step 04. Create a reference plane selecting the axis and front plane..
Step 05. Enter -30 degrees or any other degree.
Step 06. Create an axis referencing the new work plane and top work plane.
Step 07. Create a new work plane referencing the work plane and axis just created. Enter 15 degrees or any other degree.
You've just created a reference plane which you can now use to set a custom camera view.
Step 08. Select the new reference plane, right click, and select Look At.
Step 09. Make invisible any work features you'd like to ignore. My preference is to leave visible the origin reference planes.
Step 10. Save the camera view by right clicking the nearest corner of the view cube and select Set current view as home > Fit to view.
Voila! Now when you select home, the view will defualt to your new axonometric view.