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changing parameters

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Message 1 of 16
James__S
633 Views, 15 Replies

changing parameters

I have looked at the fx parameters as i want to change the Chamfer1 (fx.d5 & fx.d6) so that i can place a fillet on the nut....how do i decrease the face size so that i can use a small size fillet on the nut

JS

15 REPLIES 15
Message 2 of 16
JDMather
in reply to: James__S

Set d5 and d6 to 95% of the face width value (or whatever percentage you need).

 

Percentage.PNG


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Message 3 of 16
James__S
in reply to: JDMather

Thank you for solution

 

Can both the Bolt and Nut have a real thread on the part rather then an appearance thread?

Is this possible?

 

Best Regards

 

James

Message 4 of 16
mdavis22569
in reply to: James__S

You can put in a real thread ... but if you're going to do it yourself ... check out a few websites to see if it's already down to save you time. McMaster Carr has a lot of 3d fasteners available that you can download that have the threads shown. Mike

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Message 5 of 16
James__S
in reply to: mdavis22569

I wanted to see if i could learn the technique myself but i not sure how to start this.I think a coil feature would be one of the required tool but any suggestions on how to employ the technique of creating a real thread.

Cheers

JS

Message 6 of 16
mdavis22569
in reply to: James__S

here are a few ways via Youtube https://www.youtube.com/results?search_query=how+to+make+a+thread+cut+out+in+Inventor

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Message 7 of 16
JDMather
in reply to: James__S

See attached

or

try Fusion 360.


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Message 8 of 16
James__S
in reply to: JDMather

Bolt looks great

 

I am presuming the nut follows the same technique but will only require 1 coil feature

 

Thanks again

Message 9 of 16
JDMather
in reply to: James__S

Yes.

If you want more precise geometry (I have sharp V at OD (and at the root, but that is less of a concern)) consult your Machinery's Handbook.  Also, if you are going to 3D Print I chase a second thread offset a bit to increase clearance as the 3D Printing processes are not precise.


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Message 10 of 16
James__S
in reply to: JDMather

I thought i would post back with the 2 examples.

Is this Nut thread correct to suit the Bolt?

How do i now constrain these so that they do not interfere with each other in assembly mode?

 

eg....The assembly attached is constrained but there is interference?

 

Maybe it cannot be used this way and cosmetic threads will be better

 

Thanks

Message 11 of 16
JDMather
in reply to: James__S

Note that you did not fully cut the helix.

You must send the cutting tool all the way through the part - just like the real world.

 

Thread Cut.PNG

 

Also - the Helix in your Nut part is running CCW where it should be CW.  (Check the preview helix - don't assume the icon arrows are same axis direction as your design intent.)

 

Section View.PNG

 

 

Remember the board drawing exercise from the last century - when you section nut the back side threads appear in opposite direction from the fastener.  I always had trouble visualizing this back on the drawing board. Now you can cut it in half and see.

 


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Message 12 of 16
JDMather
in reply to: JDMather

See why the rotation axis was flipped relative to viewer.

 

Opposite Axis.png


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Message 13 of 16
James__S
in reply to: JDMather

Thanks for the help

 

It now all works.

 

Just curious why was the dimension 1.9999mm used on the triangle / coil sketch instead of 2mm?

 

Thanks

 

JS

Message 14 of 16
Paul-Mason
in reply to: JDMather

In reply to your comment "Just curious why was the dimension 1.9999mm used on the triangle / coil sketch instead of 2mm?"

 

If you use the exact 2mm thread pitch and use a 2mm coil pitch you'll get an error that the coil is self intersecting. It the same with almost, if not all, physical modeled  threads.

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Message 15 of 16
JDMather
in reply to: James__S


@James__S wrote:

 

Just curious why was the dimension 1.9999mm used on the triangle / coil sketch instead of 2mm?

 


Ha!  Old habits die hard.  I just remembered that Autodesk changed the sweep behavior in 2014 to be more forgiving of self-intersecting "errors".  I just changed it to 2mm and rebuild-all and no error.

 

I need to try this in SolidWorks and Creo now as I have had to use the same fudge in the past in those programs as well.


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Message 16 of 16
James__S
in reply to: JDMather

Thanks all for the help

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