Analyze Interference (Inspect Tab > Interference Panel in 2010; Tools menu in 2009) is perhaps one of the most commonly used commands at the end of the design process for Inventor models. The command itself is pretty straight forward, but that doesn't mean I don't get questions from time to time on it. So in this post we will look at a tip and some understanding of what the Analyze Interference command entails.
When the command is initiated, you are prompted for two sets to define interference between. This is where our tip comes in. The user does not need to pick two distinct sets for analysis. Just start clicking away and then select okay. No need for the second set button even though the arrow stays the menacing RED color. Either way will still show you the interferences in your model.
Once OK is selected you will see a red highlight on screen of all the modeling overlap in your design. This is important to discuss as some of the overlaps may be intended just as press fit dowels or other parts. Some overlap may not be desired such as a vendor part that was designed around or unforeseen constraint offset error in assembly. Perhaps one of the most questioned interferences are when they are seen on threaded holes. This we will take a deeper look at considering there is a way around it but has its own consequences.
Interference is detected here for good reason in my opinion. It is designed to show you that you did design a threaded and not a clearance hole where you wanted. Now on large machines that might not be a very clear thing to see in your analysis. Imagine you have 600-1000 bolts in your design. This would cause quite a cluttering of red on your screen. In that scenario use the Level of Detail Rep for suppression of Content Center components to ease the red devils. If you are renegade and don't use the Content Center then you will quite a bit of more work on your hands. Hey that's two tips in one post, oh how I spoil you guys. If you are of the latter inclination the next step may prove to be your savior here, but it is not without it's own drawbacks since it changes the actual modeling behavior of your parts.
Every Part has its own Document Settings as I am sure you know by now. If not, I will be covering it in an upcoming Inventomization post. But there is one setting in here that we are looking at and that is the Tapped Hole Diameter setting.
With this setting you can change the Hole size calculation to define the diameter to either the default Minor Dia, Pitch Dia, Major Dia, or Tap Drill Dia. For those rusty on the terminology...Minor Diameter is your diameter to the root or bottom of the thread, Major Diameter is your diameter to the crest or top of the thread, and Pitch Diameter is the diameter between the crest and root. There is also an option here to apply these to changes to Legacy holes (holes already created in the model).
When anything other than Minor is chosen you will be prompted that the Drawing Manager only creates acceptable threads when Minor is chosen. I have images below that show some of the differences with this. The top image is the normal Minor option and the lower image is the Major option which provides no Red Interference but does create a less technically correct documentation. With this knowledge you can apply your company methods to whichever works best for your models.
Minor Diameter option above
Major Diameter option below
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