Threaded hole call out on both sides of through hole

RobinBG

Hi there,

I am trying to define a thread on both sides of a  through hole in a boss (I don't need the thread to be the full length of the hole).
I have defined the tapped hole on both sides of the boss with apparent success in the part studio, but the thread is only showing on one side in the drawing. Is there a way to do it as I want?



Thanks for your help.

RobinBG

@PeteYodis, Thank you, I have seen the support ticket has been marked as an improvement request which confirms a work around is required in the meantime. Or just accepting a thread the whole way.

@wayne_sauder, @bryan_lagrange, thanks for the workaround - I have now shorten the tapped holes so that they don't fully intersect, and joined them by an extrude with a diameter a few ten-thousandth smaller than the drill size that Onshape uses in the hole command.

An extra step would be to hide the edges in the drawing as even if the dimension is rounded up it would still show, as it does in Wayne's document. Bryan, I suppose you have done that.


The last niggle is that the hole depth isn't correct in the hole call out, I don't think the call out can be can be manually edited but a note can be used instead. Not perfect but the drawing does end up the way I want it.

Thanks all,

Robin

Alex_Kempen

I assume it isn't working as expected because the second hole isn't actually creating any geometry; thus, it isn't actually setting its attributes. One method to fix it would be to make each hole go halfway through (at the cost of your end condition being weird); you could also make your cylinder as two halves, add the hole to each half with end condition through all, and then boolean the two halves together after.

RobinBG

Hi Alex,

Thanks for getting back to me on this.

I have tried the first method you describe already, without success - somehow as soon as the holes fully connect I loose the thread in the drawing.
Just tried to model 2 halves and do a Boolean union with no more luck, I still end up with the thread sowing on only one side on the drawing.

I originally thought the same, that my second hole feature was not actually creating any geometry, but this make me think that it is a "call out" issue from the drawing rather than a "3D" problem.

Cheers,
Robin

PeteYodis

@RobinBG This is an issue on the hole feature side and not the drawing side.  Drawings just catch the callout written for holes and don't generate them on their own.  Our hole table in the part studio is consistent with drawing hole callouts because of this.  

I've generated a ticket and we can discuss there.  

wayne_sauder

The only workaround I found, use a sketch and extrude to put a hole in your part set the dim. for the hole a few ten-thousandth smaller than the drill size that Onshape uses in the hole command.   
https://cad.onshape.com/documents/82f3542a1f94e3144be6654e/w/47fcdd67538a8d0ee1e614b7/e/74fde080cd87413774f977c3

bryan_lagrange

I did similar to @wayne_sauder having the tapped hole going to the depth needed, mirror the hole then revolve cut with a .0005 smaller hole size the area.

RobinBG

@PeteYodis, Thank you, I have seen the support ticket has been marked as an improvement request which confirms a work around is required in the meantime. Or just accepting a thread the whole way.

@wayne_sauder, @bryan_lagrange, thanks for the workaround - I have now shorten the tapped holes so that they don't fully intersect, and joined them by an extrude with a diameter a few ten-thousandth smaller than the drill size that Onshape uses in the hole command.

An extra step would be to hide the edges in the drawing as even if the dimension is rounded up it would still show, as it does in Wayne's document. Bryan, I suppose you have done that.


The last niggle is that the hole depth isn't correct in the hole call out, I don't think the call out can be can be manually edited but a note can be used instead. Not perfect but the drawing does end up the way I want it.

Thanks all,

Robin