I've had occasations when I've needed to drill a deep hole straight. One that comes to mind is when building my v8 I had to drill for the camshaft 5 inches deep and the hole had to run truly parallel to the crank shaft. Well it didn't and I still don't know how to manage a deep hole. Any suggestions?
Need help drilling a straight hole
- Thread starter jpeter
- Start date
Help Support Home Model Engine Machinist Forum:
doc1955
Gone
- Joined
- Aug 26, 2009
- Messages
- 1,261
- Reaction score
- 163
Clear the chips often (peck drill) and when reengaging material don't bang drill into bottom of hole. Every time you bang a drill into the material it will walk off center line. On deep holes depending on size I'll drill under size and if I have an end mill under the finish size I will use it to straighten hole. Deep small holes can be a real pain but if you are very careful and not push to hard clear chips often and not bang the bottom they will come out reasonably straight.
PS if you are on a mill be sure machine head is trammed in I've see people wonder why their hole isn't straight only to find that the machine head is not trammed in. And be sure to use a good center drill to start your hole.
PS if you are on a mill be sure machine head is trammed in I've see people wonder why their hole isn't straight only to find that the machine head is not trammed in. And be sure to use a good center drill to start your hole.
hammers-n-nails
Well-Known Member
- Joined
- Mar 22, 2009
- Messages
- 206
- Reaction score
- 0
in this case would it have been possible to drill both of the end journals and build a simple line-boring rig for the intermediates?
- Joined
- Feb 17, 2008
- Messages
- 2,326
- Reaction score
- 440
Sometimes it is not possible to drill a deep straight hole. The material may prevent it.
A few years ago I was rebuilding the piston valves on a Gauge 1 locomotive. The manufacturer had done a very nice job of cylindrical grinding the piston part but the sleeve was a push fit had a terrible surface finish. I decided to put cast iron liners in and lap them to fit the existing piston. These liners needed to be about 5/16 OD with a 4mm hole for the piston. No problem as I had the correct size drill and reamer.
Cast iron on hand was 1 inch diameter Class 40 gray iron. Well going from 1 inch to 5/16 inch sure makes a lot of cast iron chips and I wanted to make 4 parts, two for repair and 2 spares for another locomotive. Took a suitable length of 1 inch and quartered it so I had 4 pie shaped lengths large enough to get the 5/16 OD out of with plenty to spare. Turned them up round with the 4 jaw chuck then put them in a collet a cleaned up to length.
OK, first part. center drilled, drilled and reamed and removed from collet to do the lapping operation after I did the next three. Looked at the far end and the hole came out about 0.020 off center. Well I am still OK as I really only need 2 right now. Maybe I screwed up something. Next part I checked all the lathe alignment and the resultant part was still 0.020 off center at the far end. Third part. Drilled an undersize hole about 1/4 inch deep and opened it up to the drill size with a small boring bar. Same result as before after drilling and reaming. The hole was a nice curved hole, but quite consistent about how much off center the exit point was. So now I am down to one blank and I needed 2 parts.
About this time the light comes on. I had gotten the same result 3 times in a row. The cast iron was varying in density/hardness from the center to the outside and the drill was pulling toward the softer side. OK, I have a big vacuum cleaner for dust pick up so starting with a 1 inch diameter I turned it down to my required OD. Then into the collet as same center drill/drill/ream procedure as before. I could not measure any runout on the exit hole.
What does that have to do with your crankcase you ask? Well maybe nothing, but thinking back to when Tony (Cobra428) was building his Whittle V8 he had to make several crankcases as I recall to get his camshaft hole to run straight. I had done the same crankcase a few months before and I had no problem. While I did not think of it at the time, I think he was using extruded barstock, and I had used cast 6061 tooling plate that had been heat treated and ground so it would not warp during machining. I don't know, but suspect that the camshaft hole was near one edge of the stock and that residual stresses in the material was causing the hole to wander on his.
Like I said, I don't know if this has any bearing on your problem, but it might stimulate some other thoughts.
Gail in NM
A few years ago I was rebuilding the piston valves on a Gauge 1 locomotive. The manufacturer had done a very nice job of cylindrical grinding the piston part but the sleeve was a push fit had a terrible surface finish. I decided to put cast iron liners in and lap them to fit the existing piston. These liners needed to be about 5/16 OD with a 4mm hole for the piston. No problem as I had the correct size drill and reamer.
Cast iron on hand was 1 inch diameter Class 40 gray iron. Well going from 1 inch to 5/16 inch sure makes a lot of cast iron chips and I wanted to make 4 parts, two for repair and 2 spares for another locomotive. Took a suitable length of 1 inch and quartered it so I had 4 pie shaped lengths large enough to get the 5/16 OD out of with plenty to spare. Turned them up round with the 4 jaw chuck then put them in a collet a cleaned up to length.
OK, first part. center drilled, drilled and reamed and removed from collet to do the lapping operation after I did the next three. Looked at the far end and the hole came out about 0.020 off center. Well I am still OK as I really only need 2 right now. Maybe I screwed up something. Next part I checked all the lathe alignment and the resultant part was still 0.020 off center at the far end. Third part. Drilled an undersize hole about 1/4 inch deep and opened it up to the drill size with a small boring bar. Same result as before after drilling and reaming. The hole was a nice curved hole, but quite consistent about how much off center the exit point was. So now I am down to one blank and I needed 2 parts.
About this time the light comes on. I had gotten the same result 3 times in a row. The cast iron was varying in density/hardness from the center to the outside and the drill was pulling toward the softer side. OK, I have a big vacuum cleaner for dust pick up so starting with a 1 inch diameter I turned it down to my required OD. Then into the collet as same center drill/drill/ream procedure as before. I could not measure any runout on the exit hole.
What does that have to do with your crankcase you ask? Well maybe nothing, but thinking back to when Tony (Cobra428) was building his Whittle V8 he had to make several crankcases as I recall to get his camshaft hole to run straight. I had done the same crankcase a few months before and I had no problem. While I did not think of it at the time, I think he was using extruded barstock, and I had used cast 6061 tooling plate that had been heat treated and ground so it would not warp during machining. I don't know, but suspect that the camshaft hole was near one edge of the stock and that residual stresses in the material was causing the hole to wander on his.
Like I said, I don't know if this has any bearing on your problem, but it might stimulate some other thoughts.
Gail in NM
Mostly do what has been suggested above.
Even minor errors can cause big problems on deep holes.
Use a good (new) centre drill, drill and ream (bore if possible) pilot hole.
On a lathe make sure your tailstock is in perfect alignment. On a mill clock to the pilot hole after reaming - the assumption that it is on the same centre as your spindle just because that was where it was when you drilled might be false - especially when drilling into a centre "pop".
Ken
Even minor errors can cause big problems on deep holes.
Use a good (new) centre drill, drill and ream (bore if possible) pilot hole.
On a lathe make sure your tailstock is in perfect alignment. On a mill clock to the pilot hole after reaming - the assumption that it is on the same centre as your spindle just because that was where it was when you drilled might be false - especially when drilling into a centre "pop".
Ken
GailInNM said:
I was just reading something about this property of 7075-T6 aluminum the other day. The plates they are talking about are thick, so I wonder how much variation there is in thinner material. Alumec is a special aluminum for molds with more consistent hardness through the thickness.
https://www.alcoa.com/mill_products/catalog/pdf/commercial_rolled_products/en/Alumec_Brochure_EN.pdf
Greg
- Joined
- Feb 17, 2008
- Messages
- 2,326
- Reaction score
- 440
Greg,
That brochure has some very interesting information in it. The graphs on page 6 showing the hardness varying from about Brinnell HB 125 to 155 through out a 6 inch section of 7075 really caught my eye. I had not seen that information before.
I may have to sacrifice a two inch long, or thereabouts, section of 6061 of 1 inch square and drill and ream 5 quarter inch holes length wise in it. One in the center and and one in each corner a quarter inch in in both x and y directions. That should put the corner holes in the steepest part of the curve. Should be easy to measure any deflection by using gauge pins in each hole and see if the holes drift in a consistent pattern comparing the entrance dimension to the exit dimensions. Got my curiosity up now. Should be easy to check by measuring the holes relative to each other. If it's a problem the corner holes should drift toward the center of the stock.
Gail in NM
That brochure has some very interesting information in it. The graphs on page 6 showing the hardness varying from about Brinnell HB 125 to 155 through out a 6 inch section of 7075 really caught my eye. I had not seen that information before.
I may have to sacrifice a two inch long, or thereabouts, section of 6061 of 1 inch square and drill and ream 5 quarter inch holes length wise in it. One in the center and and one in each corner a quarter inch in in both x and y directions. That should put the corner holes in the steepest part of the curve. Should be easy to measure any deflection by using gauge pins in each hole and see if the holes drift in a consistent pattern comparing the entrance dimension to the exit dimensions. Got my curiosity up now. Should be easy to check by measuring the holes relative to each other. If it's a problem the corner holes should drift toward the center of the stock.
Gail in NM
Material stress is an interesting one. I didn't know it occurred in brass until one day I sawed down the length of some flat bar and saw either side bent out like a banana.
My usual routine is peck drilling followed by boring, sometimes with a carbide end-mill hole-straightening thrown in along the way (similar to boring, but less accurate and a lot faster), plus lots of luck. Long thin holes aren't much fun. The "Gun Drill" guys have a different tip geometry and also nearly always rotate the work instead of the drill.
My usual routine is peck drilling followed by boring, sometimes with a carbide end-mill hole-straightening thrown in along the way (similar to boring, but less accurate and a lot faster), plus lots of luck. Long thin holes aren't much fun. The "Gun Drill" guys have a different tip geometry and also nearly always rotate the work instead of the drill.
Could you not part-drill the hole with a slightly smaller drill to the depth your boring bar can reach, bore it to the size of the drill you are taking right through to make a nicely concentric 'guide' hole then continue drilling right through? Might help to keep the deeper hole on it's line.
Peter, thats an idea.
Think about this: I'm thinking drill a deep pilot hole. Next, drill to final size with an end mill, in the mill, as deep as reasonable. That'll act as a guide for the next operation which is to make a single flute drill on the end of a piece of drill rod. Drill with that cleaning often with compressed air. The drill rod would be stiffer and be guided by the end mill drilled hole. I think it's worth an experiment.
Think about this: I'm thinking drill a deep pilot hole. Next, drill to final size with an end mill, in the mill, as deep as reasonable. That'll act as a guide for the next operation which is to make a single flute drill on the end of a piece of drill rod. Drill with that cleaning often with compressed air. The drill rod would be stiffer and be guided by the end mill drilled hole. I think it's worth an experiment.
Jim,
This is what I had to do to solve a production problem.
http://bbs.homeshopmachinist.net/showthread.php?t=41213&highlight=deep+drilling
Use a ball nosed end mill, not a centre or spotting drill. You do not say whether you are on a mill or a lathe. On a mill, tramming is everything, folowed by the fit of the quill. On a lathe, drill smaller from both sides, then use a long enough size drill to go all the way through. It is still a pain in tough materials.
Ian
This is what I had to do to solve a production problem.
http://bbs.homeshopmachinist.net/showthread.php?t=41213&highlight=deep+drilling
Use a ball nosed end mill, not a centre or spotting drill. You do not say whether you are on a mill or a lathe. On a mill, tramming is everything, folowed by the fit of the quill. On a lathe, drill smaller from both sides, then use a long enough size drill to go all the way through. It is still a pain in tough materials.
Ian
Yeah, that's not a great geometry. I had to do something similar on the breech block of a Gatling-- not quite so deep (4") and I could go a bit over 3/8" dia, so I was able to use a long 3/8" carbide mill as a boring bar to straighten the hole, then reamed again to get final size.jpeter said:
