By Luke Davenport
Checking for interference in your Inventor assembly.
This is a classic case of ‘simple when you know how’. I’m sure I can’t be the only one who has used the ‘Analyze Interference’ tool incorrectly and found it slightly confusing to figure out. Hopefully this will help….
Where is it? In Inventor 2015 the tool is located on the ‘Inspect’ tab.
If you click it you’ll get a dialogue asking you to Define Set 1 and Set 2.
A couple of things to be aware of here:
1) If you define 2 sets of components they will be interference checked against each other (all of the components in set 1 will be checked against all the components in set 2).
2) If you define only a single set (and then click ‘OK’) all the components you picked will be clash checked against each other.
3) You can’t drag a box to select multiple components, you have to pick components one at a time. This is annoying to say the least.
So far so clunky. However, the simple tip here is that you need to select the components before you hit the Analyze Interference button. If you do this the analysis starts straight away and checks all the parts you picked against each other. So this then makes it very simple to analyse a whole assembly in one click.
When the analysis has finished you’ll get each interference highlighted in red on the model like this.
And you’ll also get a dialogue like this:
Expand it and you’ll get something like this, showing some info about the clash parts and clash volumes. Unfortunately this doesn’t allow individual highlighting of the clash results one-by-one. A future improvement by Autodesk perhaps?
This dialogue also can’t be resized, but will allow you to copy the table of results to the clipboard (for pasting into Excel for instance) and print the table if you like.
Taking it to the next level:
But if you have a very large assembly, why not take advantage of some of the selection options before using the Analyze Interference tool? Let’s say I want to check all these Hex bolts in the assembly to ensure that the tapped and clearance holes for them are correct. What’s the best way to do that? Well here’s one idea:
1) Switch your selection options to ‘Part Priority’
2) Right click on the bolt, and hit Selection -> Select All Occurrences.
3) We now have all the instances of this bolt in the entire assembly selected. Then right click (in empty space) again, and hit Selection -> Constrained To
4) We have now additionally selected all the components this bolt is inserted into.
5) You can repeat step 3 to select components that are constrained to the components that are constrained to the bolt. Nice.
6) Now click ‘Analyze Interference’.
7) When viewing the results, I’ll get lots of results like this, which will be ok (this is simply the thread interference). (As a small aside, setting the Tapped Hole Diameter to display as Major instead of Minor in Document Settings in a part file will remove Thread interferences like this – but as you’d probably need to switch this back afterwards (for drawing display etc.) this isn’t something you’d want to do manually often!)
But what about if I get an interference like this?
This is showing me that the clearance hole in the plate is too small for the bolt to pass through, and additionally the bolt head is buried in the plate. Needs correcting.
And what about this one?
You can just make out that this bolt is too long for the tapped hole and needs replacing. Very nice.
A couple of other tips:
1) Be aware that any parts that are not visible will not be included in the interference check. Use this to your advantage by switching visibilities to work through large assemblies step-by-step if required.
2) Also – you can drag a cross section plane through your model ahead of running the interference check to make viewing the results easier. Any parts that are partially visible will still be included in the interference check, but completely invisible parts will not.
Hope you find this useful!