Thanks!
270 Offy
- Thread starter mayhugh1
- Start date
-
- Tags
- 270 offenhauser offy
Help Support Home Model Engine Machinist Forum:
About that cam timing vernier ...
The camshaft gear has 40 teeth and, since it turns at half the speed of the crankshaft, each tooth is equivalent to 720/40 = 18 crankshaft degrees which is too coarse for meaningful valve settings. A part of Ron's camshaft design is a vernier that increases the timing resolution from 18 degrees to 4.5 degrees.
A flange at the end of the camshaft is drilled with a circular hole pattern containing four holes spaced 90 degrees apart. This flange seats inside a recess in the cam gear which is drilled with an eight hole pattern having the same bolt circle diameter. The holes in the cam gear are spaced 46.125 degrees (with 37.125 degrees left over between the last pair). The difference, in cam gear degrees, between adjacent pairs of flange holes is 92.25 - 90 = 2.25 cam gear degrees which is the new resolution i.e. one quarter of a cam gear tooth).
A pin inserted through one of the holes in the cam gear and into one of the holes in the flange selects one of four possible camshaft orientations available within that single cam gear tooth. With the crankshaft rotated into position for the timing adjustment, the camshaft is rotated so a pin can be inserted into the best-fit hole pair and then secured with one of the special nuts.
Eight flange holes could have also been used to increase the resolution by another factor of two. A point of diminishing returns is eventually reached due to errors in the actual locations and diameters of the holes, and so Ron may have felt little was to be gained beyond four.
I machined all the engine's gears several months ago from common blanks made and tested at that time. I missed the 46.125 degree spacing requirement for the cam gears discussed in the final assembly section of the manual and mistakenly drilled them 45 degrees apart. Fortunately, I had several extra gears left over from the original blanks and was able to re-drill three new cam gears from the original blanks. - Terry
The camshaft gear has 40 teeth and, since it turns at half the speed of the crankshaft, each tooth is equivalent to 720/40 = 18 crankshaft degrees which is too coarse for meaningful valve settings. A part of Ron's camshaft design is a vernier that increases the timing resolution from 18 degrees to 4.5 degrees.
A flange at the end of the camshaft is drilled with a circular hole pattern containing four holes spaced 90 degrees apart. This flange seats inside a recess in the cam gear which is drilled with an eight hole pattern having the same bolt circle diameter. The holes in the cam gear are spaced 46.125 degrees (with 37.125 degrees left over between the last pair). The difference, in cam gear degrees, between adjacent pairs of flange holes is 92.25 - 90 = 2.25 cam gear degrees which is the new resolution i.e. one quarter of a cam gear tooth).
A pin inserted through one of the holes in the cam gear and into one of the holes in the flange selects one of four possible camshaft orientations available within that single cam gear tooth. With the crankshaft rotated into position for the timing adjustment, the camshaft is rotated so a pin can be inserted into the best-fit hole pair and then secured with one of the special nuts.
Eight flange holes could have also been used to increase the resolution by another factor of two. A point of diminishing returns is eventually reached due to errors in the actual locations and diameters of the holes, and so Ron may have felt little was to be gained beyond four.
I machined all the engine's gears several months ago from common blanks made and tested at that time. I missed the 46.125 degree spacing requirement for the cam gears discussed in the final assembly section of the manual and mistakenly drilled them 45 degrees apart. Fortunately, I had several extra gears left over from the original blanks and was able to re-drill three new cam gears from the original blanks. - Terry
- Joined
- Jan 17, 2009
- Messages
- 1,081
- Reaction score
- 278
Yap, when you said the word vernier I guessed the hole pattern was not symmetric despite the difficulty from detecting it from the picture.
That is something to keep in mind building another engine. I could have easily done that on my radial, where there was ample space on the ring-gear/cam-disk interface to make a high resolution vernier.
That is something to keep in mind building another engine. I could have easily done that on my radial, where there was ample space on the ring-gear/cam-disk interface to make a high resolution vernier.
Terry: I have tried to explain the vernier idea to other builders of this engine in years past. Very few people have been able to grasp the concept on their own. Your explanation of it is excellent. Great job as usual!
Richard Hed
Well-Known Member
- Joined
- Nov 23, 2018
- Messages
- 2,380
- Reaction score
- 615
Whoa! I have been having to refer to Machineries Handbook all the time for this info on the calculator. What a pain that is. Thanx for this.
I first saw this on my 1962 Alfa Romeo twin camshafts. Wow I thought this is cool.
But forgot to use it on my own engines. Thanks for the reminder.
But forgot to use it on my own engines. Thanks for the reminder.
Jan Dressler
Member
Porsche "Fuhrmann" engines (4 cylinder horizontal opposed "Boxer", quad camshaft) used two bevel gear driven horizontal shafts to drive the lower camshafts of each cylinder bank, then two vertical shafts driving the upper camshaft from the lower one on each side.
Besides it is not very trivial to adjust those 8 bevel drives (the ones on the lower camshafts each having two pinions meshing with the same gear on the camshaft), timing adjustments are made by changing the positions of the pinions on the splined shafts, using a similar vernier system... Only that it is possible on both ends of the 4 shafts, and timing adjustments for the lower camshafts affect the upper ones as well, so have to be "reversed" if you don't want a change there.
Each of these adjustments means that you have to take apart everything again - And in the end, the adjusting possibilities are still so crude that if you want to be correct to 1° you have to use offset keys for the cams (each cam is keyed to the shaft).
In the end, I did make a whole model of the camshaft drive including cams, rockers and valves in CAD to simulate what changes are needed to achieve the correct valve timing. Still, you better keep the doors locked when working on these engines...
Somehow back to topic, incredible work on the Offy! I am a long time lurker here, but these threads are an inspiration really.
Besides it is not very trivial to adjust those 8 bevel drives (the ones on the lower camshafts each having two pinions meshing with the same gear on the camshaft), timing adjustments are made by changing the positions of the pinions on the splined shafts, using a similar vernier system... Only that it is possible on both ends of the 4 shafts, and timing adjustments for the lower camshafts affect the upper ones as well, so have to be "reversed" if you don't want a change there.
Each of these adjustments means that you have to take apart everything again - And in the end, the adjusting possibilities are still so crude that if you want to be correct to 1° you have to use offset keys for the cams (each cam is keyed to the shaft).
In the end, I did make a whole model of the camshaft drive including cams, rockers and valves in CAD to simulate what changes are needed to achieve the correct valve timing. Still, you better keep the doors locked when working on these engines...
Somehow back to topic, incredible work on the Offy! I am a long time lurker here, but these threads are an inspiration really.
I curved the flanks of my cam lobes so I can use non-keyed flat top followers. Sketches of the lobes, which are otherwise identical to Ron's, are in the photos. His documentation mentions the option of undercutting the cams to compensate for lost motion created by valve clearance in order to match the specs of the full-size cam. I selected the flanks' radii and centers to achieve a similar result with a slightly more aggressive valve opening.
The lobes were machined on my Tormach using a rotary machining operation. This 4-axis operation keeps the center of an end mill in contact with the tool path during coordinated moves of the x, y, z, and A axes. Unfortunately, the end mill's dished cutting face leaves grooves in the non-flat areas of the part. With the tool continuously moving up and down, the effect is similar to trying to drill flat holes with an end mill. The tool leaves excess material behind at its center which, in a four axis operation, shows up as a pair of grooves on either side of the cutter. Although they can be cleaned up with a file, they can be several thousandths deep depending upon the particular cutter.
These grooves can be nearly eliminated with a truly flat-bottom cutter. A local tool grinder reground a couple of my 1/4" end mills to use with this same operation during my Merlin build. However, the flat center-cutting edges are vulnerable to chipping and excessive wear, and the tool can quickly lose its advantage. To increase its lifetime, I roughed in the lobes with a conventional end mill and saved the fragile cutter for the finishing passes.
One of the photos shows two pairs of test lobes that I machined into a piece of scrap 1144 with this operation. One pair was machined using a conventional end mill and the other using the flat bottom cutter. The lobes machined with the flat tool are directly off the mill while the lobes machined with the conventional cutter received a few minutes of filing before I remembered to take the photo. Grooves created by the flat bottom tool are plainly visible (and felt) but easily removed with abrasive paper.
Each lobe pair was machined using a minimum amount of rotary axis stick-out. Although a tailstock was part of the setup, the long skinny shafts required additional support below the cutter. Since the stick-out had to be re-adjusted for each lobe pair, a simple degree wheel attached to the tailstock end of the shaft was used to reinitialize the starting angle for each lobe cutting operation.
I made up some sanding sticks to finish the lobes' surfaces by gluing abrasive paper to wood craft sticks. These are quick and easy to make by the handfuls, and they helped avoid altering the machined contours.
The lobes and bearings will be lubricated by oil pumped through the camshafts. Twelve #70 holes supply oil to these surfaces on each camshaft. They were manually drilled using a sensitive drill feed and a simple custom V fixture for support. A stream of compressed air kept the drill and hole free of the 1144's chips which tended to become magnetized and make an already difficult operation even more risky. Finally, the shafts' ends were threaded and plugged. The front plugs were drilled through with a #78 drill in order to supply oil to the cam gears.
Three of the four original blanks wound up as completed camshafts, and so I now have a spare intake cam. (Some late night carelessness resulted in one of the shafts being sliced in half.) Measurements were taken and recorded for each lobe on each camshaft. The diameters of both the heels and the heights of the noses vary +/_.003" around their mean values. These measurements will be needed later because the Offy doesn't use lash adjusters. In the full-size engines, the lengths of the valve stems were filed to adjust clearances. The manual mentions a .005" valve clearance which may be what results when everything in the valve train exactly matches the documentation. In my case, an assortment of followers will likely be required. - Terry
The lobes were machined on my Tormach using a rotary machining operation. This 4-axis operation keeps the center of an end mill in contact with the tool path during coordinated moves of the x, y, z, and A axes. Unfortunately, the end mill's dished cutting face leaves grooves in the non-flat areas of the part. With the tool continuously moving up and down, the effect is similar to trying to drill flat holes with an end mill. The tool leaves excess material behind at its center which, in a four axis operation, shows up as a pair of grooves on either side of the cutter. Although they can be cleaned up with a file, they can be several thousandths deep depending upon the particular cutter.
These grooves can be nearly eliminated with a truly flat-bottom cutter. A local tool grinder reground a couple of my 1/4" end mills to use with this same operation during my Merlin build. However, the flat center-cutting edges are vulnerable to chipping and excessive wear, and the tool can quickly lose its advantage. To increase its lifetime, I roughed in the lobes with a conventional end mill and saved the fragile cutter for the finishing passes.
One of the photos shows two pairs of test lobes that I machined into a piece of scrap 1144 with this operation. One pair was machined using a conventional end mill and the other using the flat bottom cutter. The lobes machined with the flat tool are directly off the mill while the lobes machined with the conventional cutter received a few minutes of filing before I remembered to take the photo. Grooves created by the flat bottom tool are plainly visible (and felt) but easily removed with abrasive paper.
Each lobe pair was machined using a minimum amount of rotary axis stick-out. Although a tailstock was part of the setup, the long skinny shafts required additional support below the cutter. Since the stick-out had to be re-adjusted for each lobe pair, a simple degree wheel attached to the tailstock end of the shaft was used to reinitialize the starting angle for each lobe cutting operation.
I made up some sanding sticks to finish the lobes' surfaces by gluing abrasive paper to wood craft sticks. These are quick and easy to make by the handfuls, and they helped avoid altering the machined contours.
The lobes and bearings will be lubricated by oil pumped through the camshafts. Twelve #70 holes supply oil to these surfaces on each camshaft. They were manually drilled using a sensitive drill feed and a simple custom V fixture for support. A stream of compressed air kept the drill and hole free of the 1144's chips which tended to become magnetized and make an already difficult operation even more risky. Finally, the shafts' ends were threaded and plugged. The front plugs were drilled through with a #78 drill in order to supply oil to the cam gears.
Three of the four original blanks wound up as completed camshafts, and so I now have a spare intake cam. (Some late night carelessness resulted in one of the shafts being sliced in half.) Measurements were taken and recorded for each lobe on each camshaft. The diameters of both the heels and the heights of the noses vary +/_.003" around their mean values. These measurements will be needed later because the Offy doesn't use lash adjusters. In the full-size engines, the lengths of the valve stems were filed to adjust clearances. The manual mentions a .005" valve clearance which may be what results when everything in the valve train exactly matches the documentation. In my case, an assortment of followers will likely be required. - Terry
- Joined
- Jun 4, 2008
- Messages
- 3,285
- Reaction score
- 630
Did your CAM generate the tool paths/g-code? I had come up with a way to do it via a self-written Java program and a DXF of the lobe, but haven't needed to actually do the work.
What would be the result using an endmill > 2x lobe width, offset so center never comes into play?
What would be the result using an endmill > 2x lobe width, offset so center never comes into play?
The operation I used was part of my CAM software. It was Sprutcam's first entry into the 4-axis market 13 years old and has probably been greatly improved since. The 'beta+'
version that I'm using is pretty primitive.
I think the wider the tool, the better the result. My Merlin's lobes were 1/8" wide and needed much less cleanup than the Offy's .2" wide lobes. The Knucklehead's lobes were 1/16" wide and needed no cleanup. I believe the cutting edges in the dished center of an end mill are at a 1 degree or so angle, and so will always be an error with a conventional end mill. It can be made smaller, though, with a larger diameter cutter. A torus type end mill should also help. To be honest, I'm not entirely sure why my truly flat cutter still leaves marks unless it's a combination of tram and a-axis errors.- Terry
- Joined
- Jun 24, 2010
- Messages
- 2,359
- Reaction score
- 931
Terry, re the sanding sticks, I used to do them onsey-twosey as required. But I like using them so now make them batch mode. I spray a sheet or half sheet of wet-dry paper with 3M adhesive, lay it abrasive side down on a cutting mat. Then just press the coupon stick down on it, cut directly to the edge with Exacto so the paper is flush. Flip & do the other side. I use thinner Popsicle sticks just to use up scraps of the stickied paper, but they are kind of hit & miss quality IMO. Some are not quite as flat as they appear and/or have a bit of curvature. The wider tongue depressors are worse.
So then for a period I was using strips of MDF or hardboard which is hard, smooth & cheap. But those kinds of wood can swell if it gets liquid saturated or even a bit of cutting oil. And when you remove the paper to re-use it can , it can peel back a bit of wood or leave glue residue so you have to touch it up a bit. So my latest method is nicely fly cut 3/16" aluminum strips about 1" wide x 3/16 thick. I made about 10 of them. They make a real accurate backing & any glue is readily removed with solvent & one of those plastic razor blade thingy's. Then away you go again.
When I made the valves for my radial I found the 'full width' really helped get the finish & diameter consistently across the length (work-in-progress pic). After that I decided more aluminum sanding sticks were warranted,
If you want a softer feel for feathering over gentle curves, you can use the same concept with velco stock to the tool. Then just buy hook & loop paper. Unfortunately you have to look a bit harder for wet/dry type paper suited to metal vs. woodworking (disc sander) paper. And lowest price is more predominantly circles (for disc sanders) which nets shorter sticks. Food for thought.
So then for a period I was using strips of MDF or hardboard which is hard, smooth & cheap. But those kinds of wood can swell if it gets liquid saturated or even a bit of cutting oil. And when you remove the paper to re-use it can , it can peel back a bit of wood or leave glue residue so you have to touch it up a bit. So my latest method is nicely fly cut 3/16" aluminum strips about 1" wide x 3/16 thick. I made about 10 of them. They make a real accurate backing & any glue is readily removed with solvent & one of those plastic razor blade thingy's. Then away you go again.
When I made the valves for my radial I found the 'full width' really helped get the finish & diameter consistently across the length (work-in-progress pic). After that I decided more aluminum sanding sticks were warranted,
If you want a softer feel for feathering over gentle curves, you can use the same concept with velco stock to the tool. Then just buy hook & loop paper. Unfortunately you have to look a bit harder for wet/dry type paper suited to metal vs. woodworking (disc sander) paper. And lowest price is more predominantly circles (for disc sanders) which nets shorter sticks. Food for thought.
Attachments
- Joined
- Jan 17, 2009
- Messages
- 1,081
- Reaction score
- 278
I like the brass support in the middle.
- Joined
- Dec 31, 2010
- Messages
- 777
- Reaction score
- 195
Terry:
I'm wondering about your choice of cutter diameter when you are milling the cam lobes. I believe with a finished cam the diameter of the lifter is important otherwise the geometry of how the lifter follows the cam is impacted. Too small and the edge of the lifter contacts the cam. Not sure if too large also has issues.
I'm wondering if the same would be true when you are machining the cam with what is essentially the same geometry as a lifter. Is it possible the cams are over / under cut due to the diameter of the cutter? What consideration do you have for the size of the cutter?
After finishing a cam lobe have you ever tried setting up a dial indicator with a nose the same diameter as your planned lifter. Rotate the cam keeping track of rotational degrees (using the A-axis rotary on you mill) and actually measure the opening / closing degrees and lift / duration to see if the lobe acts as designed?
I've played around with this a lot and have found the lobes are not exactly as expected. They are "close enough". I can't account for where the error occurs.
Thanks
I'm wondering about your choice of cutter diameter when you are milling the cam lobes. I believe with a finished cam the diameter of the lifter is important otherwise the geometry of how the lifter follows the cam is impacted. Too small and the edge of the lifter contacts the cam. Not sure if too large also has issues.
I'm wondering if the same would be true when you are machining the cam with what is essentially the same geometry as a lifter. Is it possible the cams are over / under cut due to the diameter of the cutter? What consideration do you have for the size of the cutter?
After finishing a cam lobe have you ever tried setting up a dial indicator with a nose the same diameter as your planned lifter. Rotate the cam keeping track of rotational degrees (using the A-axis rotary on you mill) and actually measure the opening / closing degrees and lift / duration to see if the lobe acts as designed?
I've played around with this a lot and have found the lobes are not exactly as expected. They are "close enough". I can't account for where the error occurs.
Thanks
- Joined
- Jan 17, 2009
- Messages
- 1,081
- Reaction score
- 278
This is an issue it has always bugged me, and have not quite formulated a clear understanding.
Is easy enough to specify a cam in polar coordinates.
For every angle: machine an infinitesimal angle at a specific distance from the center, with a an infinitesimal tool diameter. Theoretical, but this is just to establish the geometry.
If the lifter had an infinitesimal diameter (an indicator ball) then the lift profile as read by the indicator would match the specification.
BUT
A real cutter does also cut "ahead" into the yet to be machined part of the cam. Will the cam be over cut when we come to machine the next location? Or there will still be metal to shave away.
A small roller lifter "reads" the cam on a vertical radial bit a large flat lifter "reads" the cam on a radial that is not vertical but at the point where the tangent is horizontal.
I understand that Terry concerns with the tool shape are not related, the groves are anomalies in the axial extension of the cam.
One alternative could be to use the side of the end mill which will cut straight even a wide cam. But that is only possible with a single cam, impossible on a long shaft with multiple cams.
- Joined
- Dec 31, 2010
- Messages
- 777
- Reaction score
- 195
I think you are re-iterating pretty much what I was saying.
"The proof is in the pudding" as they say. That's why I asked if he has ever checked the specs on the cams after machining them using the actual lifter (or if a flat lifter with a flat tip on the indicator the same diameter). I have, and although I don't machine them this way mine don't come out exactly as expected.
BTW I grind them with a very large (8" dia) grinding wheel so it's sort of the same but different
.
The process of taking tangent cuts as per the old camcalc program seems to be very good but it leaves a bit of filing to get rid of the facets. Then after filing where does that leave you??
This is why machining cams is a bit of a black art. The machining process has to take into account all of those little things.
Yes side milling seems to be (probably) a more accurate scheme because the cam program takes into account the diameter of the cutter. An inside profile is a good example. They come out perfectly regardless of shape as long as the cutter is not too large for an inside corner. I have made cams this way making pairs of lobes held in a fixture. But then the pairs need to be assembled on a shaft. Sort of a pain.
When ground on a professional machine the pattern the grinding wheel follows IS NOT just a large diameter version of the finished cam.
It's a bit of a black art.
"The proof is in the pudding" as they say. That's why I asked if he has ever checked the specs on the cams after machining them using the actual lifter (or if a flat lifter with a flat tip on the indicator the same diameter). I have, and although I don't machine them this way mine don't come out exactly as expected.
BTW I grind them with a very large (8" dia) grinding wheel so it's sort of the same but different
.The process of taking tangent cuts as per the old camcalc program seems to be very good but it leaves a bit of filing to get rid of the facets. Then after filing where does that leave you??
This is why machining cams is a bit of a black art. The machining process has to take into account all of those little things.
Yes side milling seems to be (probably) a more accurate scheme because the cam program takes into account the diameter of the cutter. An inside profile is a good example. They come out perfectly regardless of shape as long as the cutter is not too large for an inside corner. I have made cams this way making pairs of lobes held in a fixture. But then the pairs need to be assembled on a shaft. Sort of a pain.
When ground on a professional machine the pattern the grinding wheel follows IS NOT just a large diameter version of the finished cam.
It's a bit of a black art.
Last edited:
I've never checked the cams for accuracy other than with a degree wheel in the engine when it came time for setting the timing. This only involved checking the opening and closing times and the locations of the lobe centers. And yes they've always been, as you say, 'close enough'.
When one has four axes to work with, there are a multiple combinations of axis movements that can cut the same profile. I've always been curious about how CAM programs make this choice especially since I was thinking about making one of my own before this operation was released.
The software I have assumes it is working with a truly flat cutter (which in most cases it's not), and it keeps the center of that cutter in contact with the tool path. During the tool path calculations, any movements that might gouge the part are checked for and disallowed. You can watch the extra movements that are inserted in order to avoid the "cutting ahead" gouges that Mauro talks about. When running, the A-axis isn't just turning continuously while the z-axis moves up and down. The A-axis often pauses and sometimes reverses while the y-axis makes some back and forth movements of its own. I've always assumed it was doing this to avoid gouging the part with the cutter's front edge. The whole process is pretty interesting to watch. Sometimes when making these movements, however, the depth of cut is greater than the conservative value that I typically enter into the parameter list, and it is probably here that my truly flat cutters are susceptible to damage.
I wouldn't think commercial cams for any application are cut with end mills. Rotary cutters and grinding wheels avoid the problems that I run into. I don't know if my 13 year old CAM software was ever improved to avoid this issue or if there is another way of using what I do have to work around it. For example, there is an option to keep the front of the cutter in contact with the tool path instead of its center, but I've never gotten that option to compile my particular version. - Terry
When one has four axes to work with, there are a multiple combinations of axis movements that can cut the same profile. I've always been curious about how CAM programs make this choice especially since I was thinking about making one of my own before this operation was released.
The software I have assumes it is working with a truly flat cutter (which in most cases it's not), and it keeps the center of that cutter in contact with the tool path. During the tool path calculations, any movements that might gouge the part are checked for and disallowed. You can watch the extra movements that are inserted in order to avoid the "cutting ahead" gouges that Mauro talks about. When running, the A-axis isn't just turning continuously while the z-axis moves up and down. The A-axis often pauses and sometimes reverses while the y-axis makes some back and forth movements of its own. I've always assumed it was doing this to avoid gouging the part with the cutter's front edge. The whole process is pretty interesting to watch. Sometimes when making these movements, however, the depth of cut is greater than the conservative value that I typically enter into the parameter list, and it is probably here that my truly flat cutters are susceptible to damage.
I wouldn't think commercial cams for any application are cut with end mills. Rotary cutters and grinding wheels avoid the problems that I run into. I don't know if my 13 year old CAM software was ever improved to avoid this issue or if there is another way of using what I do have to work around it. For example, there is an option to keep the front of the cutter in contact with the tool path instead of its center, but I've never gotten that option to compile my particular version. - Terry
- Joined
- Jun 4, 2008
- Messages
- 3,285
- Reaction score
- 630
Given that a cam lobe is convex, a flat tool tangent to any point can't touch any other point. So I don't understand why gouging could come into play as long as the path keeps the tool tangent to the intended surface. The A axis should be able to move continuously.
Similar threads
