-
Welcome back Guest! Did you know you can mentor other members here at H-M? If not, please check out our Relaunch of Hobby Machinist Mentoring Program!
[How-To] Pecking. For drilling, yes; how about for reaming?
- Joined
- Sep 1, 2020
- Messages
- 549
Like John I don’t think in terms of in/min for drilling since I am doing all manual. I can estimate that if I was reaming a 3/8” hole 1.250” through it would only take me about 15-20 seconds tops and be easily double likely triple my drilling rate. So if drilling 2 in/min then I would guess about 5 in/min for the reamer and that calculates out to ¼ minute or 15 seconds. Would seem about right for my manual mind.
- Joined
- Dec 20, 2012
- Messages
- 9,422
Like all tools, reamers work best when continually cutting but there is a catch. Reamers can only take off about 0.005" or less without losing accuracy. If you look at the chart David linked, the pre-reamer drill is about that, 0.005" less than the reamer. A reamer can actually straighten a slightly crooked hole up to this 0.005" limit so pay attention to your drill size.
The material you're reaming also makes a difference. If the material is harder, drill even closer to the final reamer size because the reamer cannot take off as much. You also have to slow your speed in harder stuff.
Speeds matter. I know there are reamer speed recommendations all over the place but I tend to run reamers slow, somewhere in the 100-200 rpm range. The reason for this is because I can feel the reamer cutting as I feed in; if I go faster I lose that feel.
Feeds differ according to the material as well. Harder material require slower feeds and vice versa. This is where a manual machinist has an advantage for one-off stuff because he is going by feel. What you're looking for is a slight resistance as you feed the reamer into the hole and you have to maintain it so the tool cuts continuously. Push too fast and the reamer may deflect; push too slow and you burnish the cutting edges and dull your tool.
If all else fails, you can always bore it.
The material you're reaming also makes a difference. If the material is harder, drill even closer to the final reamer size because the reamer cannot take off as much. You also have to slow your speed in harder stuff.
Speeds matter. I know there are reamer speed recommendations all over the place but I tend to run reamers slow, somewhere in the 100-200 rpm range. The reason for this is because I can feel the reamer cutting as I feed in; if I go faster I lose that feel.
Feeds differ according to the material as well. Harder material require slower feeds and vice versa. This is where a manual machinist has an advantage for one-off stuff because he is going by feel. What you're looking for is a slight resistance as you feed the reamer into the hole and you have to maintain it so the tool cuts continuously. Push too fast and the reamer may deflect; push too slow and you burnish the cutting edges and dull your tool.
If all else fails, you can always bore it.
- Joined
- Mar 26, 2018
- Messages
- 8,408
Good information.Like all tools, reamers work best when continually cutting but there is a catch. Reamers can only take off about 0.005" or less without losing accuracy. If you look at the chart David linked, the pre-reamer drill is about that, 0.005" less than the reamer. A reamer can actually straighten a slightly crooked hole up to this 0.005" limit so pay attention to your drill size.
The material you're reaming also makes a difference. If the material is harder, drill even closer to the final reamer size because the reamer cannot take off as much. You also have to slow your speed in harder stuff.
Speeds matter. I know there are reamer speed recommendations all over the place but I tend to run reamers slow, somewhere in the 100-200 rpm range. The reason for this is because I can feel the reamer cutting as I feed in; if I go faster I lose that feel.
Feeds differ according to the material as well. Harder material require slower feeds and vice versa. This is where a manual machinist has an advantage for one-off stuff because he is going by feel. What you're looking for is a slight resistance as you feed the reamer into the hole and you have to maintain it so the tool cuts continuously. Push too fast and the reamer may deflect; push too slow and you burnish the cutting edges and dull your tool.
If all else fails, you can always bore it.
John mentioned a fairly aggressive feed.
For the price of a quality reamer, you wouldn’t want to damage it.
It brings up another element. If you are using a cheap drill or one that is dull or just not sharpened properly, the drilled hole could be out of spec more than .005”.(the size of the drill bit doesn’t mean that’s what you are going to end up with. Is what I’m trying to say).
The test hole is a great idea. I’ll have to remember that trick.
- Joined
- Dec 20, 2012
- Messages
- 9,422
Good point, Jeff.
I don't know about you guys but I have more trouble coming in on size with smaller reamers, under 1/4" diameter, than larger ones. Many years ago, I ran trials to figure out what technique I would use personally. While I'm sure other guys do it better, I have better accuracy doing it this way.
I choose the pre-reamer drill so it leaves as close to 0.002-0.003" of meat to be removed by the reamer. Then I choose a drill one size smaller than that pre-reamer drill and use it as a rougher. I just spot the hole and use that pre-pre-reamer drill without using pilots or step drilling. This minimizes any wandering of the hole and gives me the best chance of a straightish hole. The pre-reamer drill then only has a small amount of material to take off and this sizes the hole properly and takes off any gnarly finish that first drill produces. The reamer is next and I make a single pass without dwelling and use a fair amount of cutting fluid. Once I reach the bottom or am through the hole, I turn off the machine and withdraw the reamer. This gives me the best finish with the truest diameter. It also seems to make the reamers stay sharper longer.
I've reamed hundreds of holes this way and it works for me. Not saying you guys should do it this way but you might try it if you get stuck for a technique.
- Joined
- Jan 12, 2021
- Messages
- 14
Here is what I came up with using scraps of aluminum for testing. In all instances I used a 23/64th carbide coated drill bit.
Going straight through the hole with the reamer at 1.0 in/min the spindle bogged down a bit.
Going straight through but stopping several times without any retraction seemed to work well.
Thanks to all that contributed. It's been a useful learning experience for me.
Going straight through the hole with the reamer at 1.0 in/min the spindle bogged down a bit.
Going straight through but stopping several times without any retraction seemed to work well.
Thanks to all that contributed. It's been a useful learning experience for me.
- Joined
- Mar 26, 2018
- Messages
- 2,724
Here are my comments coming from a hobby CNC guy with a bit of experience:
1) Use a canned cycle for programming efficiency. Your CAM software should use these anyways. G83 is a peck drill cycle which is great for deep holes when you cannot get the drill to break nice chips. Full retracts to the feed plane at rapid rate. G73 is a chip break cycle that uses small retracts inside the hole to break the drill chip. It is good for when the chips are breaking nicely anyways and you want to give them some help evacuating. It is much faster than G83. In a canned cycle, you define the cycle on the first line then all subsequent positions apply the same drilling cycle until canceled by a G80. Here is an example
G83 X1 Y1 Z-1.5 R0.1 Q0.25 F10
X2 Y1
X2 Y2
X1 Y2
G80
In this case we call a peck drill canned cycle (G83) starting at X1 Y1 to a depth of Z-1.5. The drill will drill down in 0.25" increments (Q) retracting to 0.1" above the part (R). Retract in and out of the hole is done at rapid while cutting (including a bit of air cutting R distance above the previous cut depth) is done at 10 ipm (F). At each subsequent location (e.g. X2 Y1, X2 Y2, etc...) the full drilling cycle is repeated without needing to type the whole G83 string again. The canned cycle is canceled with a G80 and the machine goes back to normal movement.
2) I always drill to 97% of the reamed hole dimension (or as close as possible). I try to never go above 97% and if I cannot find a drill bigger than 94%, I will bore the hole to pre-ream diameter. This happens on bigger holes as you have fewer drill options.
3) The SFM for reamers (used to calculate spindle speed) is slow compared to drilling. HSS reamers in alloy steel for example can run in the 30-50 SFM range. For a 1/4" reamer this is 460-760 rpm. The feed is comparatively high at 0.006" per tooth. This is 16.5-27.5 in/min. You can go proportionally slower in both speed and feed as desired. Lots of charts online, take a look at this: https://www.redlinetools.com/customer/docs/RedLineToolsReamersTechInfo.pdf
4) Pecking on reamers is typically not needed, but chip packing can be a problem in holes over 6xTool Diameter (6xD) with a 97% predrill or 4xD with a 94% predrill. A peck can be added if needed.
5) Pecking can be important on blind holes at 2xD or greater as chips can get pushed to the bottom of the hole.
6) The reamer should be retracted from the hole while rotating and at the specified feedrate. EDIT: Mikey commented he shuts the spindle off so that must work too!
7) Reamer concentricity is important and should be held to <0.0005" if you are trying to make a precision hole. This can be verified with a test indicator on the cutting flutes. Out of concentricity cutters can be tapped into alignment using a mallet of soft material (lead or copper). Bell mouthed holes and chatter at hole entry are a symptom of poor cutter concentricity.
1) Use a canned cycle for programming efficiency. Your CAM software should use these anyways. G83 is a peck drill cycle which is great for deep holes when you cannot get the drill to break nice chips. Full retracts to the feed plane at rapid rate. G73 is a chip break cycle that uses small retracts inside the hole to break the drill chip. It is good for when the chips are breaking nicely anyways and you want to give them some help evacuating. It is much faster than G83. In a canned cycle, you define the cycle on the first line then all subsequent positions apply the same drilling cycle until canceled by a G80. Here is an example
G83 X1 Y1 Z-1.5 R0.1 Q0.25 F10
X2 Y1
X2 Y2
X1 Y2
G80
In this case we call a peck drill canned cycle (G83) starting at X1 Y1 to a depth of Z-1.5. The drill will drill down in 0.25" increments (Q) retracting to 0.1" above the part (R). Retract in and out of the hole is done at rapid while cutting (including a bit of air cutting R distance above the previous cut depth) is done at 10 ipm (F). At each subsequent location (e.g. X2 Y1, X2 Y2, etc...) the full drilling cycle is repeated without needing to type the whole G83 string again. The canned cycle is canceled with a G80 and the machine goes back to normal movement.
2) I always drill to 97% of the reamed hole dimension (or as close as possible). I try to never go above 97% and if I cannot find a drill bigger than 94%, I will bore the hole to pre-ream diameter. This happens on bigger holes as you have fewer drill options.
3) The SFM for reamers (used to calculate spindle speed) is slow compared to drilling. HSS reamers in alloy steel for example can run in the 30-50 SFM range. For a 1/4" reamer this is 460-760 rpm. The feed is comparatively high at 0.006" per tooth. This is 16.5-27.5 in/min. You can go proportionally slower in both speed and feed as desired. Lots of charts online, take a look at this: https://www.redlinetools.com/customer/docs/RedLineToolsReamersTechInfo.pdf
4) Pecking on reamers is typically not needed, but chip packing can be a problem in holes over 6xTool Diameter (6xD) with a 97% predrill or 4xD with a 94% predrill. A peck can be added if needed.
5) Pecking can be important on blind holes at 2xD or greater as chips can get pushed to the bottom of the hole.
6) The reamer should be retracted from the hole while rotating and at the specified feedrate. EDIT: Mikey commented he shuts the spindle off so that must work too!
7) Reamer concentricity is important and should be held to <0.0005" if you are trying to make a precision hole. This can be verified with a test indicator on the cutting flutes. Out of concentricity cutters can be tapped into alignment using a mallet of soft material (lead or copper). Bell mouthed holes and chatter at hole entry are a symptom of poor cutter concentricity.