01-02-2014, 10:18 AM
I hope this does not get too long - but what you are undertaking is not a trivial task. I don't have any quick and definite answers - but here's some guidelines on how to do the drawing(s).
The Atlas-Clausing engineering department probably had at least two drawings to describe this part:
1) A drawing of the rough casting - which was used to make the pattern for the foundry work
2) A drawing of the machining work on the casting
Am I correct to guess that the part will be made from a piece of bar stock rather than a casting? If so, both the drawing technique and the machining technique will be different from the original part. The real difference will be that the initial set-ups and work on the critical dims can be done with stock that is pretty much flat and square - easy to mount in a vice or clamp to the table. (Working on a raw casting usually took some special set-up efforts). If it were me, I would want to do the drilling and boring while the part was still a rectangular block - then, add the "casting" features after the critical work is done.
So I am thinking two drawings.
1) Dwg 1 shows the critical holes, bosses and bores applied to rectangular shaped part.
2) Dwg 2 shows whatever of the casting features you think you want to add to make the part look somewhat original.
For Dwg 1, both you and the machinist get to dimension and work from 3 perpendicular planes x,y,z (you only get to use 3, the other 3 surfaces of the stock just come along for the ride and are never referenced). This portion of the machining work can easily be done on a manual mill. You get to describe, dimension and tolerance the critical dims without having all the casting features in the way. For my taste, I think this drawing is 5 views with a section cut of the "U" slot. The 5 views (using the names you have already started) are Front, Left, Right, Bottom, and Back. The Section View is an abbreviated cut perpendicular to the axis of the U slot with just enough Dims to show the location and width of the U. Since the Section is a "cut" you get to conveniently show the surface of the bore as an "elevation" reference to the center of the radius of the slot.
For Dwg 2, CNC will be the easiest machining technique, if available. Otherwise a lot of hand grinding and fitting will be required. The good news is that few, if any, of the casting features such as drafts and radii are critical. This drawing also has several views with one or two sections to show the different casting features. Since most of these features are not critical, you can describe one feature and then state that the same feature is "Typical" on all of the part. This works well for convex radii, concave radii and for drafts. The square reference planes will disappear as this portion of the work is done, so all of the dims need to be referenced back to features that were generated in the first drawing (bores and bosses). Don't include any of the Dims from Dwg 1 on Dwg 2 unless they really need to be there for the machinist to reference (and then label the dimension as "Ref" so he knows that there is nothing to be done for this dim).
Be aware that different countries interpret the L-R and Top-Btm views differently. If a fellow DownUnder is doing the work, this will not be a problem. German drawings (and maybe a few others) are backwards from the American system.
One of the drafting challenges will be getting the critical dimensions off of the existing part in a way such that the accuracy can be preserved on the drawing. The boss, the c-bore and the hole for the rotating shaft all need to be concentric to some degree. The machinist gets to make two of these features on one set-up (without flipping the part), so decide which of the two are more critical and dimension them together with a concentricity tolerance (+- .001 is not out of line here). For the 3rd feature, which requires flipping the part, dimension from the center of the hole (which can be indicated after the part is flipped). Here, +-.001 is asking for a lot of indicating, so decide if you can give him +- .002 or whatever. In both cases, the concentricty tolerance is separate from the diameter tolerance.
Likewise, the distance from the center of the boss and c-bore to the center of the bore for the plunger is probably critical. You will have to take some measurements on a flat surface (granite or machine table), with the plunger installed. Take measurements in every possible way and then do some math to see if they agree with one another. Also keep in mind that the original designer probably selected an "even" number for this dimension. So if you come up with 1.502, the original part was probably designed at 1.500.
I have worked with draftsmen who would sketch up a part like this by hand and then send through the machine shop without issues. You are probably going to work with a drafting table or a CAD program. If you are a CAD wizard (and the machining will be CNC), you could generate a database to build the part - but that's a lot of work and I think unnecessary in this case. But, basic CAD technique will force you to do some work that will confirm if the measurements you took from the part make sense.
Here are a few of my other notes for what they are worth:
The old rule pounded into draftsmen from the early days, is that the drawing needs to be presented in the way that the part will be fabricated. The draftsman has to have enough machining knowledge to describe the features and dimensions in a way that will make sense to the machinist. Describe the critical dimensions first, and the least critical last. Don't include dimensions that have no use to the machinist. Never "double dimension" - if you do this, the machinist never knows which dimension you actually want to "hold." Always dimension to a feature that the machinist will be able to locate accurately - and will be able to easily check for accuracy after completion. The machinist assumes that every dimension on the part will be some step in the process. Always try to dimension in a way that can be "checked" after machining. In the case of features that require some math, such as hole spacing on bolt circles, describe the feature in the standard way and let the machinist do the math, trig, use his DRO or whatever to achieve the feature. Don't ask for accuracy that you don't need. The machinist will usually deliver accuracy that exceeds the drawing tolerances, but he will welcome some "slop" that allows him to not have to re-make a part that failed on what was actually a non-critical dimension.
Terry S.
The Atlas-Clausing engineering department probably had at least two drawings to describe this part:
1) A drawing of the rough casting - which was used to make the pattern for the foundry work
2) A drawing of the machining work on the casting
Am I correct to guess that the part will be made from a piece of bar stock rather than a casting? If so, both the drawing technique and the machining technique will be different from the original part. The real difference will be that the initial set-ups and work on the critical dims can be done with stock that is pretty much flat and square - easy to mount in a vice or clamp to the table. (Working on a raw casting usually took some special set-up efforts). If it were me, I would want to do the drilling and boring while the part was still a rectangular block - then, add the "casting" features after the critical work is done.
So I am thinking two drawings.
1) Dwg 1 shows the critical holes, bosses and bores applied to rectangular shaped part.
2) Dwg 2 shows whatever of the casting features you think you want to add to make the part look somewhat original.
For Dwg 1, both you and the machinist get to dimension and work from 3 perpendicular planes x,y,z (you only get to use 3, the other 3 surfaces of the stock just come along for the ride and are never referenced). This portion of the machining work can easily be done on a manual mill. You get to describe, dimension and tolerance the critical dims without having all the casting features in the way. For my taste, I think this drawing is 5 views with a section cut of the "U" slot. The 5 views (using the names you have already started) are Front, Left, Right, Bottom, and Back. The Section View is an abbreviated cut perpendicular to the axis of the U slot with just enough Dims to show the location and width of the U. Since the Section is a "cut" you get to conveniently show the surface of the bore as an "elevation" reference to the center of the radius of the slot.
For Dwg 2, CNC will be the easiest machining technique, if available. Otherwise a lot of hand grinding and fitting will be required. The good news is that few, if any, of the casting features such as drafts and radii are critical. This drawing also has several views with one or two sections to show the different casting features. Since most of these features are not critical, you can describe one feature and then state that the same feature is "Typical" on all of the part. This works well for convex radii, concave radii and for drafts. The square reference planes will disappear as this portion of the work is done, so all of the dims need to be referenced back to features that were generated in the first drawing (bores and bosses). Don't include any of the Dims from Dwg 1 on Dwg 2 unless they really need to be there for the machinist to reference (and then label the dimension as "Ref" so he knows that there is nothing to be done for this dim).
Be aware that different countries interpret the L-R and Top-Btm views differently. If a fellow DownUnder is doing the work, this will not be a problem. German drawings (and maybe a few others) are backwards from the American system.
One of the drafting challenges will be getting the critical dimensions off of the existing part in a way such that the accuracy can be preserved on the drawing. The boss, the c-bore and the hole for the rotating shaft all need to be concentric to some degree. The machinist gets to make two of these features on one set-up (without flipping the part), so decide which of the two are more critical and dimension them together with a concentricity tolerance (+- .001 is not out of line here). For the 3rd feature, which requires flipping the part, dimension from the center of the hole (which can be indicated after the part is flipped). Here, +-.001 is asking for a lot of indicating, so decide if you can give him +- .002 or whatever. In both cases, the concentricty tolerance is separate from the diameter tolerance.
Likewise, the distance from the center of the boss and c-bore to the center of the bore for the plunger is probably critical. You will have to take some measurements on a flat surface (granite or machine table), with the plunger installed. Take measurements in every possible way and then do some math to see if they agree with one another. Also keep in mind that the original designer probably selected an "even" number for this dimension. So if you come up with 1.502, the original part was probably designed at 1.500.
I have worked with draftsmen who would sketch up a part like this by hand and then send through the machine shop without issues. You are probably going to work with a drafting table or a CAD program. If you are a CAD wizard (and the machining will be CNC), you could generate a database to build the part - but that's a lot of work and I think unnecessary in this case. But, basic CAD technique will force you to do some work that will confirm if the measurements you took from the part make sense.
Here are a few of my other notes for what they are worth:
The old rule pounded into draftsmen from the early days, is that the drawing needs to be presented in the way that the part will be fabricated. The draftsman has to have enough machining knowledge to describe the features and dimensions in a way that will make sense to the machinist. Describe the critical dimensions first, and the least critical last. Don't include dimensions that have no use to the machinist. Never "double dimension" - if you do this, the machinist never knows which dimension you actually want to "hold." Always dimension to a feature that the machinist will be able to locate accurately - and will be able to easily check for accuracy after completion. The machinist assumes that every dimension on the part will be some step in the process. Always try to dimension in a way that can be "checked" after machining. In the case of features that require some math, such as hole spacing on bolt circles, describe the feature in the standard way and let the machinist do the math, trig, use his DRO or whatever to achieve the feature. Don't ask for accuracy that you don't need. The machinist will usually deliver accuracy that exceeds the drawing tolerances, but he will welcome some "slop" that allows him to not have to re-make a part that failed on what was actually a non-critical dimension.
Terry S.