Creating Holes in Assembly Mode 1

21Pom · Nov 7, 2010

Hi All,

I have a circular fan case onto which I need to mount a terminal box support bracket and with a little bit of mucking around with the constraints I can get the bracket where I want it. What I caannot seem to do is place holes, that are already in the bracket, into the case. I can secure the bracket using some Tek Screws but what I wanted was the holes in the case so that the case Flat Pattern is laser cut from a sheet and when rolled up everything will come together.

Any ideas?

Best Rgds,
Dave R

rollupswx · Nov 7, 2010

Assembly (iam file) without parts (ipt files) is, of course, useless.

EngAddict · Nov 7, 2010

You might want to look into using a bolted connection, it will add the hole for you. Or you can use adaptivity in the part environment but I wouldn't recommend it. Best option is skeletal modelling.

21Pom · Nov 7, 2010

Hi All,

OK, attached are the ipt files that rollupswx requested.

Tried the bolted connection but the holes did not appear on the case ipt. Being fairly new at Inventor I'm still feeling my way around it so am not sure as to how work the Skeletal modeling.

Best Rgds
Dave R

21Pom · Nov 7, 2010

Hi All,

Couldn't figure out how to attach more than one file so here is the other one.

Best Rgds,
Dave R.

Gensunasumus · Nov 9, 2010

if you can att. zip file than use pack & go

rollupswx · Nov 9, 2010

I got the files - haven't had time to demo solution.
One thing I did notice the hole that was added was not correct. (look at it in flat pattern - sides not perpendicular to flat)

EngAddict · Nov 9, 2010

Here is the simplest method, see attached for 'adaptive' cross part association method. Not what I would recommend but the simplest solution without using derived parts or multi-body modelling.

Steps:
1. edit casing in the assembly.
2. create sketch on the terminal bracket face.
3. extrude the holes through the casing.
4. mirror or repeat for the other side.

21Pom · Nov 10, 2010

Hi EngAddict,

That was the bit that I could not get too, i.e., creating a sketch on the support bracket in Assembly Mode.

Once I had that all I did was Project the hole on the bracket onto the sketch and then reproduce the hole with enough length to get through the case.

Thanks for the heads up on how to get there.

Best Rgds,
Dave R.

21Pom · Nov 10, 2010

Hi rollupswx,

If I understand you correctly, the two flats where the holes are located are not supposed to be perpendicular to the sides, they are bent down towards the curvature of the case and generally follow the curve on the front vertical face.

Best Rgds,

Dave R.

rollupswx · Nov 10, 2010

Not what I was getting at, but I also wondered about your design intent on those flanges as well.

In your original cylindrical part that you attached here go to the flat pattern. Go to Wireframe view. You should only see a circle (actually ellipse) at the edge of the hole - not multiple edges. Which brings up another consideration - the hole cannot be both round in the flat and in the folded model. You need to make a decision of whether it is round in the folded (but elliptical in the flat or round in the flat and bent elliptical in the folded.

21Pom · Nov 10, 2010

Hi Rollupswx,

H'm, it seems that I need to pay a lot more attention to how I create parts using Inventor. I'm just amazed at, with just a few lines, Inventor brings things to life.

I'll go back over the parts again and see what I've done wrong - thanks for you input and concern.

Best Rgds,

Dave R.

21Pom · Nov 10, 2010

Hi rollupswx,

Yes, I see what you are getting at. What I did was to create a sketch on a plane that toched to top of the case, pin point where the hole was to go and drop a hole through the case, abviously not the way to go. I'll re-do that and hopefully I get it right next time.

Best Rgds,
Dave R.

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