how to do it ?

[dho]

the first Inventor file shows an endmill cutting, but it would be not the right way to model it. (the .25R corner next to the small hole)
the second file, used fillet radius, but it does not represent the actual part.
how to do it?
thanks.

 

[dho]

the second file.

 

[JNieman]

Pictures are probably better than Inventor part files, especially since this is an AutoCAD forum section.

I, myself, cannot open Inventor files. I expect the modeling is pretty straight forward no matter the software - so a screenshot would probably make it easier to help you.

 

[berkshire]

Can you export the file as a PDF file ?
B.E.

You are judged not by what you know, but by what you can do.

 

[dho]

first i posted in solidworks group since there is no inventor group. i was told to post in autocad group.
here are the JPG of rendered shape. file1 minics endmill cut, file2 (next thread) just a simple fillet at the corner.
without inventor to open ipt file, you may have problem to visualize the issue.
thanks.

 

[JNieman]

http://www.eng-tips.com/threadminder.cfm?pid=790

<--- Inventor Group

I agree - I can't really visualize it too well from that image.

Are you doing some weird boolean subtraction? It looks like a cylinder representing an end mill has been removed from that 'puck' shaped blank, and arrayed every so often around a different radius. It looks like an attempt to use an end mill in a vertical machining center while the part rotates under it on a 4th axis rotary. But it may be a weird rendering effect...

I don't understand the question any better from the image in the post dated 7Nov16-20:04, though, sorry.

 

[btrueblood]

It looks like you made a single cylindrical cut, then patterned it a number of times through small angular increments?

If you want the cut to be smoother, you need to do a sweep - have the cutter shape follow a path (and or guide surface) that you define with a third sketch.

 

[dho]

as said, inventor (ours 2014) will not do sweep a solid but only a 2D sketch.

 

[btrueblood]

Yes, but if you use a guide curve that is a 3D sketch (and click on the boxes to have the profile remain perpendicular to the guide curve) you can sweep a rectangular profile to cut any given radius, mimic-ing the results of a spinning cylindrical cutter.

 

[dho]

btrueblood, do you have Inventor? would you please upload a file so i can see how it works?
thanks.

 

[btrueblood]

Yes, but it's 2016. I don't know how to save a file to 2014 format.

But here is a batch of pdf files showing how I built a sweep that I think does what you want...

Start from sketch 2 - a 2d outline of the cutter (I'm going to model a .125 deep cut with a .25 diameter end mill)
sketch 3 is an arbitrary arc, concentric with the bar and on its end face
I make a plane perpendicular to the end of the arc, through the axis of the bar (which I created about the global z-axis), and create sketch 4, which is just a line perpendicular to the end of the arc.
Sketch 4 was necessary to create workplane 2, which is tangent to my sketch 3 arc.
Sketch 5 is created on workplane 2, and is a simple arc with one end coincident and tangent to the sketch 3 arc and its work plane.
The sweep is then created from the sketch #2 as the profile, and using sketch 3 and sketch 5 as the path. Note if sketch 2 had overlap beyond the edge of the part, the turn radius along the edge would be less than zero, and the sweep would fail. I.e. I can't make a complete groove deeper than the radius of the cutter with this method, but would have to do it in two sweeps or other methods.

Ok, I didn't bother to make a 3d sketch, because I don't like how inventor's 3d sketch interface works, but you get the idea.