Chamfer with taped side

[cadcamm99]

I am trying to put a chamfer on my model that has one tapered side.  I am trying to accomplish the chamfer such as the bottom right one in the chamfer definition image.  You can see the references I used in the model.  However, when I dimension the chamfer in the drawing using the chamfer button, I get the following. Is there anyway to make this work?

I also tried the dxd and d1xd2 method and that doesn't seem to work either.  If I choose the taper side as the reference then I get .107x45°

[JDMather · Accepted solution]

If you have trouble getting exactly what you want with Chamfer - you could always Sweep (or extrude) a triangle with the exact dimensions you want.

If you have trouble figuring it out - attach your *.ipt file here.

[Mario428]

From a manufacturing perspective "what difference"?????  Why would you insist on dimensioning a chamfer to 3 places of decimal? Using 2 places makes it .10. I could get into the use of a chamfer where a radius would be much easier to machine or create but I won't.  LOL

The chamfer dimension measures the length of the line and bacause of your tapered part it is longer then .100, the chamfer is created by moving the edge .100 in each direction along the face. Edit feature to .096 and it will be .100 on your drawing.

[Cadmanto]

It looks like you are trying to put in a weld fillet.

If that is the case try this function.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[cadcamm99]

I figured that is what I would have to do.  I wish they had the option to flip the angle to the reference side.  It seems the angle comes off the taper side which is wrong.  If it came off the reference side then it would come out correct.  If I use the tapered side as the reference then it is the opposite and I end up with a .107 dim.  Thanks.

[Mario428]

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@cadcamm99 wrote:

I figured that is what I would have to do.  I wish they had the option to flip the angle to the reference side.  It seems the angle comes off the taper side which is wrong.  If it came off the reference side then it would come out correct.  If I use the tapered side as the reference then it is the opposite and I end up with a .107 dim.  Thanks.

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If you did a sketch using a couple of .100 long line and a hypotenue at 45 degs to each line you would see why your hypotenuse

length works out the way it does depending on the reference face.

The vertical face gives a .104 long Hypotenure and the angled face gives a .107 long hypotenuse, pretty basic geometry

[cadcamm99]

That is if I am using dxd or d1xd1 but I am using dx45° like in the chamfer definition. However, inventor does not take the angle off the reference side.  It takes it from tapered side.

See attachment.  This is what comes up when I Show Dimensions in the model.  This is wrong. If the 45° came off the horizontal reference then it would be correct.  But since it comes off of the tapered side, I get .104 in the drawing.

[Mario428]

Just showing how Inventor creates a chamfer, it is scaled up 10-1 to more easily show the geometry.

Take note of the perpedicular line that makes it 1.000, angles line makes 1.036 or the .104 you came up with.

Same sketch referenced off the angle face would be .107 long