Hi All,

Can anyone assist in solving this little problem.  I have a 20mm cube on which I have drawn 20mm circles on 3 sides, for this question, I hope to have the circles on all sides.

Where the corners of the cube meet is where I want to chamfer that point back to the circles, if you know what I mean.  I tried having the circles 1mm thicker than the cube and then using fillet, push back the sides of the cube, but that didn't work.

Got any ideas?

Best Rgds,
Dave R.

You mention both fillet and chamfer which leaves it unclear to me what you are after (see attached).
Also - I noticed that none of your sketches are constrained - you might start here http://home.pct.edu/~jmather/skillsusa%20university.pdf
 

• http://files.engineering.com/getfile.aspx?folder=3477f6da-c74d-47dd-9292-9d

Hi rollupswx,

Sorry about the confusion, I tried both methods is what I meant.  I'll have a look at the link and get back to you.

Thanks for your quick response.

Beast Rgds,
Dave R

Hi Rollupswx,  I looked at the link you offered and I've seen that before in a slightly different form, it did not help me.

As for the file you sent, I cannot open it mainly because I forgot to inform you of my version of Inventor.  It is 2011 Professional and I beleive the file you are sending is 2012?

Best Rgds
Dave R

Quote:

I looked at the link you offered and I've seen that before in a slightly different form, it did not help me.

If you can't figure out how to constrain simple sketches, you are correct - I can't help you.

Quote:

As for the file you sent, I cannot open it mainly because I forgot to inform you of my version of Inventor.

Surely you understand that a *.png is an image file and not an Inventor part file.  Good luck!

Hi rollupswx,

Two things,

1/  I do know how to constrain sketches but miss read your comment and thought it was a link showing how to construct what I was after.

2/  I tried to open the file in photoshop but it refused so I assumed wrongly that it was an Inventor file.

I may not be the sharpest tool in the box by any means but I do try and even before I ask for help I do spend some time trying to complete the problem.  I finally opened your file using Windows Photo View.  The top part of the image appears to be what I'm after.

Rgds,
Dave R.

1 constrained sketch
1 extrude
1 revolve
(see attached image file)

• http://files.engineering.com/getfile.aspx?folder=4ad877be-fd20-454c-8037-05

Maybe we can take this step-by-step.
Create a 4-sided polygon at the origin as shown.
Attach the file here.

• http://files.engineering.com/getfile.aspx?folder=d7bf055c-72bd-4141-b623-77

Hi rollupswx,

The image you sent before is exactly what I'm after.  I spent several hours yesterday and into the evening trying to get it without success, it was only after I slept on it that I finally got it.  I think it was the revolution part that put me on the right track although I'm absolutely certain that my effort will be by far inferior to yours.

How I finally approached it was to create a sphere and then create 20mm circle sketches on various planes which I then cut extruded out from there.  It is a very long winded way to aproach the problem so, in my interest of learning more about Inventor, I would greatly appreciate the step-by-step approach you took.

Rgds
Dave R.

Quote:

I would greatly appreciate the step-by-step approach you took.

You are going to laugh when you see how easy it really is.
Attach your square sketch part here as previously instructed.

Hi rollupswx,

I'll probably laugh with shame.  I had this before on something, can't think what it was now, and when I saw how easy it was I felt such a fool.

OK got the polygon in place.

Rgds, Dave R

Hang on, forgot to attach file
 

• http://files.engineering.com/getfile.aspx?folder=f842f17b-f3e1-46a0-a2af-ac

It appears that you are still doing too much work - get lazy.
Create the square using the polygon tool.
Set to 4 sides and click the origin and any distance away.
Add one horizontal constraint to any one of the lines.
Add the 20mm dimension.
Done with that sketch.

Hi rollupswx

OK done that - see attached.

Rgds,
Dave R

• http://files.engineering.com/getfile.aspx?folder=9eb0a40d-972f-4733-9b5b-2e

I would have added the horizontal constraint only to a line - not to midpoint and origin.  The reason is covered in that document I linked earlier. Doesn't really matter for this case - but it is all about developing rock-solid techniques that never fail in an case.

Start Sketch2 and Project Geometry the 3 corner points shown with red arrows.  Sketch the arc and diagonal line shown in red.
 

• http://files.engineering.com/getfile.aspx?folder=6a077c63-8fb9-480e-acc9-59

Extrude Sketch1 midplane (now called symmetric) and click on the 20mm dimension to set that as the extrude distance.

• http://files.engineering.com/getfile.aspx?folder=d50c8de6-7abd-4671-a522-9a

Revolve the arc in Sketch2 and select Intersection as the Boolean result.

 

• http://files.engineering.com/getfile.aspx?folder=c33a6e0f-3bd4-434d-bb88-ba

Hi rollupswx,

I don't know about laughing, I'm just shaking my head in amazement.  That's brilliant!!  Well I would never had worked that out. Like I said, it puts my effort to shame in no uncertain terms. It certainly opens up a whole new area to explore and see what else one can discover.

Once I got the idea of revolving the circle that inscribed the square I started to get some where in my own feeble way.

I again take my hat off to you and thank you for your help.

Rgds,
Dave R