Why do my circle dimention's differ from the 3D model to the 2D?

[gschmidt73]

I modelled a small .750" x 8" axle. I started my sketch as a .750" diameter circle, modelled the axle with 3/4" length of 3/4-16 threads for the first 3/4", there's a small keyway approximately 2/3 down with 2 crossed drilled hole's towards the other end. 

When I drew my 2D sketch from the 3D model, it tell's me the shaft is .745" so my question is where did the .005" go?

Also why are my small holes measuring .188" and .25" when I made them .1875" and .250"?

I have no problem with the hole spacing measurement which is 1.492"

I've redrawn the circle a few times, even tried drawing it as .755" to see if anything would change but still reads .745"

I'm assuming its operator error as i'm still green and have a long ways to go, looking for some advice..

Thank you,

George

[jhackney1972]

The Thread feature remodels the shaft diameter to match the major diameter, which is taken from the thread tables.  This is a application design flaw that has been submitted many time before.  The best way around this problem is to create a thread relief where the shaft thread ends, this will prevent the Thread feature from modifying the un-threaded section of the shaft.

[jeff_strater · Accepted solution]

applying threads will modify the diameter of the cylinder to which they are applied.  I can never remember which value is used (nominal, etc), but that is applied to the whole cylinder.  To apply it only to the threaded part, use Split Face at the point where the threads end, then apply the thread.  Only the thread portion will be modified, the rest should still be .75.  Sample model attached

[gschmidt73]

Thanks Jeff, I tried using the split face but wouldn't work, so I tried the split body...worked perfectly, I learnt something new today, much appreciated! 

[jhackney1972]

By using the Split Body command you now have two bodies in your component, will that give you issues?

[TheCADWhisperer]

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@gschmidt73 wrote:

Thanks Jeff, I tried using the split face but wouldn't work,

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@gschmidt73 

You want to resolve why it did not work for you.

I recommend that you attach the file that did not work.

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[g-andresen]

Hi,

After the situation with the reduced shaft diameter was described here some time ago, I took another look at various screws from different suppliers and found that they all had a reduced shaft diameter compared to the nominal size.

günther

[TheCADWhisperer]

@g-andresen 

manufactured massed produced threads are usually rolled threads (metal displacement - stronger) rather than cut threads.

In my experience Cut threads (as opposed to rolled threads) are generally done on max diameter stock. Perhaps with an undercut as suggested by @jhackney1972 

[jeff_strater]

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@gschmidt73 wrote:

Thanks Jeff, I tried using the split face but wouldn't work, so I tried the split body...worked perfectly, I learnt something new today, much appreciated! 

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@gschmidt73 - did you look at the file I shared?  Split Face seemed to work OK for me.  I tested without splitting, and I did see the change from .75in to .744 in when I applied the thread.  After the Split Face, the part of the cylinder to which the thread was applied was .744, but the part below the split remained at .75

You can absolutely use Split Body, but that requires an extra step:  Combine to put the cylinder back together.