AnsweredAssumed Answered

Dimensioning Hole Depth

Question asked by Wing Hoe Tan on Feb 25, 2018
Latest reply on Sep 15, 2020 by Dave Laban

Like • Show 0 Likes0
Comment • 8

Hi all, a general question to all engineers out there regarding dimensioning of hole depth in drawings. In hole wizard, the hole depth is defined as the distance from the surface to the cylindrical edge (5 mm in the example) below. If you measure from the tapered point, the depth is slightly more at 5.75 mm.

In the hole callout, do you specify 5 mm or 5.75 mm? Is there a universal convention for this? How do machinists interpret the callout?
Is it customary to provide a detailed cross-section to prevent confusion?

Tony Tieuli Feb 26, 2018 6:59 AM

Correct Answer

Wing Hoe Tan wrote:

Hi all, a general question to all engineers out there regarding dimensioning of hole depth in drawings. In hole wizard, the hole depth is defined as the distance from the surface to the cylindrical edge (5 mm in the example) below. If you measure from the tapered point, the depth is slightly more at 5.75 mm.
In the hole callout, do you specify 5 mm or 5.75 mm? Is there a universal convention for this? How do machinists interpret the callout?
Is it customary to provide a detailed cross-section to prevent confusion?

As a rule I would dimension that drilled hole depth to 5mm.

As a machinist I would interpret the depth of the drilled hole to 5mm unless I saw the words "To drill tip" in which case I would interpret the depth to be 5.75mm..If the depth was dimensioned to the drill tip I would also expect the angle of the drill tip to be specified.

See the reply in context

No one else had this question

Outcomes

Solid Air Feb 25, 2018 11:44 PM

Where I work, dimension goes to bottom of hole not drill point

Actions

Kevin Pymm Feb 26, 2018 3:21 AM

Generally the dimension goes to the bottom of the full diameter of the hole, not the point as Solid Air says. In some cases it might be important to dimension the end of the point to prevent break through of a part but I would still dimension the depth of the hole & maybe specify the angle of the drill point.

In this link you will find very few, if any, examples that dimension to the point.

Actions

Tony Tieuli Feb 26, 2018 6:59 AM

Wing Hoe Tan wrote:

Hi all, a general question to all engineers out there regarding dimensioning of hole depth in drawings. In hole wizard, the hole depth is defined as the distance from the surface to the cylindrical edge (5 mm in the example) below. If you measure from the tapered point, the depth is slightly more at 5.75 mm.
In the hole callout, do you specify 5 mm or 5.75 mm? Is there a universal convention for this? How do machinists interpret the callout?
Is it customary to provide a detailed cross-section to prevent confusion?

As a rule I would dimension that drilled hole depth to 5mm.

Actions

Husein Delic Feb 26, 2018 7:14 AM

1. You should always set the drill depth to the full diameter end not the end point like in your case 5.75mm (only special case where the drill angle needs to be different or it close to a wall to add a note). So 5mm is the right one.

2. On such simple hole callouts I never set a section drawing. A callout like on second image is enough for machinist to get it right done. But on some advanced hole cutouts I would suggest to add section and show important dimension to get away from any confusions that could come up!

Actions

Wing Hoe Tan Feb 26, 2018 7:51 AM

Hi all, thank you for the feedback. In the course of my design work, I am often faced with drill hole depths that are close to the panel thickness. I always have a fear of machinists interpreting the depths wrongly and drilling all the way through. For these cases, it looks like it will be better to provide a dimensioned cross-section. For typical cases, I will dimension to the cylindrical depth. Thanks again.

Actions

Dave Laban @ Wing Hoe Tan on Sep 15, 2020 3:30 AM

Wing Hoe Tan wrote:

Hi all, thank you for the feedback. In the course of my design work, I am often faced with drill hole depths that are close to the panel thickness. I always have a fear of machinists interpreting the depths wrongly and drilling all the way through. For these cases, it looks like it will be better to provide a dimensioned cross-section. For typical cases, I will dimension to the cylindrical depth. Thanks again.

You can always add a note to your drawing stating your convention for the avoidance of doubt.

Actions

Brian Herr Sep 14, 2020 5:29 PM

Interesting question.
I have experience as a CNC Programmer and machinist in addition to being a Licensed PE in Mechanical Engineering.
I general, machinists and programmers are looking at the drill tip. When you setup a machine, you indicate the drill tip. While it's possible to indicate the shoulder, it's much more difficult.

The vast majority of my blind holes are for threaded holes. With that being said, I know I need to have a clearance below the minimum required thread of 1-2 (2-3 preferred) threads for a bottoming tap. I define both the shoulder and the point in my drawings, based on a 118 deg drill bit.

That being said, Solidworks is missing a critical feature within the threaded hole feature by not allowing you to define the drill depth by the point. That way, you can quickly set your depth, and then check the available thread depth, from which you can check the stackup of components to know if you need to adjust the thickness of a washer, a mating part, the depth of a counterbore, etc. to engage the proper amount of threads.

If you don't include the tip depth, someone in the manufacturing chain will likely end up doing it anyway.

As a cheat sheet, I have a spreadsheet that gives the additional height of the tip of a drill from the shoulder.

Actions

Richard Gergely @ Brian Herr on Sep 14, 2020 9:32 PM

I agree with you Brian and I would go as far as manual drilling with DRO as well. When it gets to the machinist/toolmaker all they will be bothered about is the tip and thread depth.

Actions

8 Replies

Solid Air Feb 25, 2018 11:44 PM
Mark Correct
Correct Answer
Where I work, dimension goes to bottom of hole not drill point
Like • Show 4 Likes4
Actions
Kevin Pymm Feb 26, 2018 3:21 AM
Mark Correct
Correct Answer
Generally the dimension goes to the bottom of the full diameter of the hole, not the point as Solid Air says. In some cases it might be important to dimension the end of the point to prevent break through of a part but I would still dimension the depth of the hole & maybe specify the angle of the drill point.

In this link you will find very few, if any, examples that dimension to the point.
Like • Show 5 Likes5
Actions
Tony Tieuli Feb 26, 2018 6:59 AM
Unmark Correct
Correct Answer
Wing Hoe Tan wrote:

Hi all, a general question to all engineers out there regarding dimensioning of hole depth in drawings. In hole wizard, the hole depth is defined as the distance from the surface to the cylindrical edge (5 mm in the example) below. If you measure from the tapered point, the depth is slightly more at 5.75 mm.
In the hole callout, do you specify 5 mm or 5.75 mm? Is there a universal convention for this? How do machinists interpret the callout?
Is it customary to provide a detailed cross-section to prevent confusion?
As a rule I would dimension that drilled hole depth to 5mm.
As a machinist I would interpret the depth of the drilled hole to 5mm unless I saw the words "To drill tip" in which case I would interpret the depth to be 5.75mm..If the depth was dimensioned to the drill tip I would also expect the angle of the drill tip to be specified.
Like • Show 4 Likes4
Actions
Husein Delic Feb 26, 2018 7:14 AM
Mark Correct
Correct Answer
1. You should always set the drill depth to the full diameter end not the end point like in your case 5.75mm (only special case where the drill angle needs to be different or it close to a wall to add a note). So 5mm is the right one.
2. On such simple hole callouts I never set a section drawing. A callout like on second image is enough for machinist to get it right done. But on some advanced hole cutouts I would suggest to add section and show important dimension to get away from any confusions that could come up!
Like • Show 3 Likes3
Actions
Wing Hoe Tan Feb 26, 2018 7:51 AM
Mark Correct
Correct Answer
Hi all, thank you for the feedback. In the course of my design work, I am often faced with drill hole depths that are close to the panel thickness. I always have a fear of machinists interpreting the depths wrongly and drilling all the way through. For these cases, it looks like it will be better to provide a dimensioned cross-section. For typical cases, I will dimension to the cylindrical depth. Thanks again.
Like • Show 1 Like1
Actions
- Dave Laban @ Wing Hoe Tan on Sep 15, 2020 3:30 AM
  Mark Correct
  Correct Answer
  Wing Hoe Tan wrote:
  
  Hi all, thank you for the feedback. In the course of my design work, I am often faced with drill hole depths that are close to the panel thickness. I always have a fear of machinists interpreting the depths wrongly and drilling all the way through. For these cases, it looks like it will be better to provide a dimensioned cross-section. For typical cases, I will dimension to the cylindrical depth. Thanks again.
  You can always add a note to your drawing stating your convention for the avoidance of doubt.
  Like • Show 1 Like1
  Actions
Brian Herr Sep 14, 2020 5:29 PM
Mark Correct
Correct Answer
Interesting question.
I have experience as a CNC Programmer and machinist in addition to being a Licensed PE in Mechanical Engineering.
I general, machinists and programmers are looking at the drill tip. When you setup a machine, you indicate the drill tip. While it's possible to indicate the shoulder, it's much more difficult.

The vast majority of my blind holes are for threaded holes. With that being said, I know I need to have a clearance below the minimum required thread of 1-2 (2-3 preferred) threads for a bottoming tap. I define both the shoulder and the point in my drawings, based on a 118 deg drill bit.

That being said, Solidworks is missing a critical feature within the threaded hole feature by not allowing you to define the drill depth by the point. That way, you can quickly set your depth, and then check the available thread depth, from which you can check the stackup of components to know if you need to adjust the thickness of a washer, a mating part, the depth of a counterbore, etc. to engage the proper amount of threads.

If you don't include the tip depth, someone in the manufacturing chain will likely end up doing it anyway.

As a cheat sheet, I have a spreadsheet that gives the additional height of the tip of a drill from the shoulder.
Like • Show 2 Likes2
Actions
- Richard Gergely @ Brian Herr on Sep 14, 2020 9:32 PM
  Mark Correct
  Correct Answer
  I agree with you Brian and I would go as far as manual drilling with DRO as well. When it gets to the machinist/toolmaker all they will be bothered about is the tip and thread depth.
  Like • Show 1 Like1
  Actions

Dimensioning Hole Depth

Outcomes

Related Content

Recommended Content