 I welcome you all for module 3 lecture 4. In this lecture, we will be discussing about the various factors favoring the loose tolerances and tight tolerances. We will have the discussion on the selection of different kinds of fits and the assessment of the fit and tolerances and how we can calculate the tolerance unit value. Also, we will discuss about the geometrical tolerances. Now, I am showing few engineering parts, the bearings which require very fine finishes and very tight tolerances. We can see here, we have some bearings, ball bearings with very fine finish. So, it is very essential that we have to control the dimensions and it is also necessary that we have to control the features, geometric features. For example, the roundness, flatness, tightness, etcetera, etcetera, so that they function in a proper way. Here, we have fluid film bearings used in hard disk. We can see that they have very fine finishes with very tight tolerances, so that they function properly without much run out problem. So, they require very fine I t grades like I t 4, I t 5, etcetera, so that their functioning will be proper. Now, this table shows the factors in favor of wide and narrow tolerances, when we should go for narrow tolerances, when we should go for wider or loose tolerances. The factors in favor of loose tolerances are given below. They increase the yield in manufacturing and there will be fewer defects are produced and fabrication of toolings like dies, jigs, etcetera will be very easy. So, tools will be, they will not be very costly because of the loose tolerances. We need not have to use very precise machining processes. So, the production cost of the parts will be less and setup and tooling adjustment will be very easy if we have the loose tolerances and then fewer production operations may be needed. We need not have to go for very finer finishing processes like a lapping, etcetera, etcetera. A simple fine turning or rough grinding will be enough and the less skilled and lower cost labor can be used. If we select very tight tolerances, what happens is we have to go for the lapping process, super finishing process, diamond turning process like that. So, in such cases, we have to use very skilled operators. If the tolerances are wide, we can use semi-skilled operators so that the labor cost will be less and also the machine maintenance will be reduced and the need for inspection will also be reduced. Cost of inspection will be reduced. The reason is we can use normal measuring instruments and if we provide very tight tolerances, then we have to go for very fine precise measuring tools. So, investment on inspection cost will increase if we have tight tolerances and then overall manufacturing cost is reduced. Reason is the not so precise machines can be used and semi-skilled operators can be used and the inspection cost will reduce. So, due to this, the overall manufacturing cost also will reduce and what are the conditions favoring tight tolerances. See, when we provide very appropriate tight tolerances, the parts interchangeability is increased in assembly. That means we can randomly select the mating parts and we can easily assemble. So, which may not be possible if the tolerances are very, very loose. And then fit and finish of the assembled product will be better and the aesthetic will also be better if we have tight tolerances and then production functionality and performance will be improved and the products produced will be durable and they will be reliable in service. And the serviceability of the product in the field is likely to improve due to increased parts interchangeable. That means the components to be replaced, they are readily available in the market like bearings, belts, etcetera, etcetera, taper pins, different kinds of fasteners, they are readily available. So, we can purchase them and we can replace them. So, interchangeability aspect will improve and product will be safer to use. Now, we will move to steps in assessment of limits and fits. That means how we can assign the proper tolerances and how do we get the proper fit and how to select the proper fit. So, these are the steps followed for assessing the limits and fits. The selection of proper fits based on functional needs, that means what is the basic intention of the product, where it is used, whether running clearance is required or very tight clearance, tight fit is required or very wide tolerance and very wide clearance is required. So, depending upon the functionality, we have to select proper fits, whether we want clearance fit or transition fit or interference fit like that. So, it basically depends upon the functional needs, what is the application of the meeting parts. And then once we select the proper fits based on functional needs, within that we have to select what type of hole is required or what type of shaft is required. For example, if we select clearance fit, within that what is the hole that whether we require H hole or B hole or C hole. Similarly, when they come to the shaft, what type of shaft is required, H shaft is required or M shaft is required or B shaft is required. So, that we have to select. And then the selection of tolerance grades for hole as well as for shaft also, we have to properly select, whether we require H7 or H8 or if it is the very precise operation is required, very proper location is required, then we may have to go for I t 4, I t 5 like that. And if it is for the manufacturing of gauges used for inspection purpose, we may have to go for I t 2, I t 3 like that. So, depending upon the again based upon application, we have to select proper tolerance grades for hole as well as for shaft, which will decide the amount of the tolerance on the hole and shaft. And then we have to calculate the standard tolerance I for a particular combination and then calculation of limits on hole and shaft. That means, once we know what is the type of hole and what is the type of shaft and then what is the tolerance grade we are using and after finding the standard tolerance value, then we can fix up what is the upper limit for the hole, what is the lower limit for the hole. And similarly, what is the upper limit for shaft and what is the lower limit for the shaft, those things can be calculated. And then after once we find the limits for hole and shaft, we can calculate what is the amount of clearance, what is the maximum amount of clearance, what is the minimum amount of clearance, if it is clearance fit. And then we can if it is interference fit, what is the maximum interference, minimum interference and if it is the transition fit, what is the maximum interference, what is the minimum clearance, such things can be calculated. And once we calculate all these things, So, we can prepare the drawing, we can mention all the tolerance etcetera etcetera, and that drawing can be supplied to the manufacturing unit for the making of the products. Now, let us discuss about the selection of fits. Now, again basically the fit depends depends upon what is the application, whether the fit we have to select for the pulleys, and then motor bearings, and then heavily loaded bearings, and whether we are assigning the fit and tolerance for lubricated bearings or gear boxes, loadage shafts etcetera etcetera. So, based upon the application, we can select what is the type required, whether we can go for large clearance, loose clearance, and then normal running clearance, precision running clearance. So, once we fix up the type of fit that is needed, then we can go for what is the shaft. So, this is basically a whole basis system. So, H capital H whole is required. Now, we have to select the shaft, what type of shaft is required, whether A shaft is required, B shaft. See, when the large clearances are needed for general usage, then we go for ABC shafts, which will provide very large clearances. And then for accurate bearings, we may have to go for GE shaft, and then also depending upon application, we have to properly select what is the tolerance grade, whether 4 is required, 5 is required, 6 is required, 8 is required. So, like this, the such tables we can use for selection of fits. And preferred clearance fits are mentioned here, H11, C11, H9, D9, so and then H7, H6, like this, these are preferred. So, once we fix up the clear, what is the type of shaft and grade, then we can select the appropriate preferred, nearest preferred clearance fit. Similarly, we have tables available for selection of transition fits, again based on the whole basis system. Again, we can see there are many application are mentioned here, very accurate location, couplings, gears, and then precision joints, forced assembly sometimes may be required and semi-permanent or type fit assembly we may have to design. In such cases, we have to appropriately select the fit, slight clearance is required or very little clearance is required, that we have to find. And then we have to appropriately select the shaft, whether K is required, M is required and N is required. And then we can also select the IT grade. And then we have the preferred transition fit. So, we can select the preferred fit also. Similarly, we have interference fit. Again, some applications are mentioned here for fixing bushes, we may go for interference fit, for tight press fit and then valve seating and then permanent assemblies. So, in such cases, we go for interference fit. For example, for permanent assembly with H, capital H whole, we can use this T shaft or U shaft. And for valve seating, scholars, etcetera, we can go for S shaft with tolerance grades 5, 6 or 7. And then again, we have the preferred interference fits. We can select the type of fit out of these preferred interference fits. Now, after studying all these basics, we will see some numerical examples. I have taken an example here. We follow all the steps. For example, selection of fit and calculation of tolerance unit, etcetera, etcetera, so that the basics can be understood clearly. Now, the problem is the diameter of the shaft is 70 millimeter. That is the basic size or the design size of the shaft is 70 millimeter. And then tolerance grade is H 8 for whole and F 7 for shaft. So, H whole with I T 8 grade is used and for shaft, F shaft is used with I T 7. So, the tolerance grades and type of whole, they are already mentioned in the example. Now, what we have to do is, we have to calculate the standard tolerance unit and then whether there is any fundamental deviation. And then, what is the upper limit and lower limit for shaft? Similarly, what is the upper limit and lower limit for whole? That can be calculated. And finally, we can say whether the type of fit obtained is clearance fit or interference fit. Now, we have to find fundamental deviation, tolerances for whole and shaft and limits of size for whole and shaft. Also, we have to mention what is the type of fit. And also, we have to calculate maximum and minimum interference or maximum and minimum clearance. Depending upon fit obtained, we have to mention what is maximum interference or clearance and what is maximum type, maximum amount of these interferences and clearances. Now, the solution is given here. Calculation of standard tolerance unit. So, we can use this equation i is equal to 0.45 times cube through tough d plus 0.001 times d. So, where d is mean diameter. That means, we know that the basic size is 70 millimeter and then where it falls, in what step it falls that we have to see that we can do using table 7. 70 mm, it falls in the range of 50 to 80. So, now we can find the mean d that is cube root of I am sorry square root of 50 times 80. So, this will be equal to 63.25 millimeter. This is the value of mean diameter. Now, we have to insert this d in this equation to find the tolerance unit. So, the value of d is inserted here 0.45 times cube root of 63.25 plus 0.001 times 63.25. So, this will give us 1.865 micrometer or 0.0018 millimeter. Now, after finding this i, we can find the tolerance values for shaft and wall. Now, we are using F7 shaft. So, tolerance value for I t grade 7 is equal to 16 i. So, this we can get from table number 5. So, now the tolerance value for the shaft is equal to 16 times i, where i is equal to 0.0018 millimeter. So, this will be equal to 0.03 millimeter. Similarly, we can find the tolerance value for whole. So, we are using H whole with I t grade 8. So, tolerance value for I t 8 will be 25 i and then the i value we have already calculated that is 0.0018 millimeter. So, tolerance for shaft I am sorry tolerance for whole will be equal to 25 i that will be equal to 0.046 millimeter. Now, after finding the tolerance unit and tolerance values for whole and shaft, we can find the fundamental deviation. Since, we are using the whole basis system, the fundamental that is H whole we are using. So, fundamental deviation for whole is 0. Now, we have to find the fundamental deviation for the shaft f. Now, from the table number 4, we can get this equation for getting the fundamental deviation for f shaft. So, for f shaft fundamental deviation that is upper deviation is equal to minus 5.5 times d to the power of 0.41. So, we have to feed the value of d that is 63.25. Then, we get fundamental deviation which is nothing but upper deviation as 0.030 millimeter. So, once we find the fundamental deviation tolerance values, we can fix up the limits for shaft and whole. Now, higher limit for shaft is equal to the basic size of the shaft that is 70 millimeter minus fundamental deviation. So, that is 0.03 millimeter. So, we get higher limit as 69.97 millimeter. Similarly, for lower limit of the shaft, higher limit of shaft minus tolerance that is higher limit is 69.97 and the tolerance value for the shaft is 0.03. So, this will give us lower limit of 69.94 millimeter. Similarly, for whole we can find lower limit and for limit. So, in this case lower limit for whole is 70 millimeter. Reason is fundamental deviation is 0. That means lower limit of the whole will be equal to basic size that is 70 millimeter and higher limit can be calculated by adding tolerance to the lower limit. So, we get 70.046 millimeter. Now, we can show this graphically like this. We have a 0 line. This is a 0 line. From this 0 line, we show all the other dimensions like tolerance value, basic size, etcetera, etcetera. Now, we are using H8 whole. So, this is H8 and for H8 whole, we have calculated the tolerance value. So, tolerance for H whole is 0.046 millimeter. That is this tolerance value is 0.046 millimeters and then coming to the, this is the lower limit for the whole which is equal to the basic size 70 millimeter. Since the deviation is 0, the lower limit for the whole is equal to the basic size and we have to add this tolerance value to this basic size to get the upper limit of the whole. Then upper limit of the whole is 70.046 millimeter. This is the upper limit. Now, we have F7 shaft. So, this is F7 shaft. With the tolerance value of tolerance value for F7 shaft is 30 microns. So, this is 0.03 millimeter and also the fundamental deviation that is upper deviation. So, upper limit of the shaft is nearer to the zero line. So, this is upper deviation and we have calculated the upper deviation for the shaft that is 0.03 millimeter. Now, using this tolerance value and this upper deviation, we can fix up the limits for the shaft. So, that we have already found here, higher limit of the shaft. This is the higher limit, H limit for shaft. So, higher limit is 69.97 and then lower limit we get at this point. So, this gives us the lower limit. That means from the upper limit, we have to deduct this tolerance value. Then we obtain the lower limit. So, this is the maximum clearance. So, this gives us the maximum clearance. That means, we get the maximum clearance when the shaft size is equal to the lower limit and hole size is equal to the maximum size. Then we get the maximum clearance. So, what we have to do is, we have to add this tolerance for shaft and then we have to add this fundamental deviation and then we have to add this tolerance for hole. Then we get the maximum clearance and this difference between the minimum size of the hole and maximum size of the shaft will give us the minimum clearance that is equal to 0.03 mm. Now, we can compare these values, the shaft limits and maximum clearance, minimum clearance with the table 3. The basic size is, we are using 70 millimeter. So, we get 70 millimeter between the 60 and 80. Then we have calculated the tolerance for hole is 46 millimeter. So, we are using h 8 hole. So, we have h 8 hole here. So, now we can see here, this difference is 46 microns for 60 millimeter basic size. Similarly, we have same tolerance value for 80 millimeter basic size. So, for 70 millimeter basic size also, the tolerance value will be equal to 0.046 millimeter and similarly, for shaft, the tolerance value, we can see here is this difference is 30 microns. Similarly, for this 80 millimeter size, the tolerance value is 30 micrometer, 0.03 mm. So, for 70 also, same value will be there. Then we can also see the maximum clearance and minimum clearance. All these are clearance fits. You can see minimum clearance is 0.03 millimeter and maximum clearance is 0.106 millimeter. We can observe here. Minimum clearance is 0.03 millimeter and maximum clearance is 0.106 millimeter. Like this, we can calculate the values or if ready tables are available, we can use the ready table to fix up the limits for hole and shaft and to get the type of fit. Now, we have a special case of tree lobe. Now, in all the previous examples, what we studied is based upon the hole size and the shaft size, we get a particular type of fit. That means, if shaft is smaller than the hole, we get clearance fit. If the shaft is greater than the hole, then we get the interference fit and sometimes we get transition fit depending upon the actual size of the hole and shaft if the tolerance zones are overlapping. Now, this fit can be calculated by measuring the actual sizes of hole and shaft or if we know the tolerance zone for hole and shaft, we will come to know whether we get that clearance fit or interference fit. But sometimes what happens is, the shaft will not be circular. That means, we may get some lobes like this. So, this happens normally in centralized grinding wherein we have a supporting roll and then we have the workpiece and then we have a rest, a blade to keep the workpieces and then we have the grinding wheel. So, if the workpiece setting is not proper or the blade height is not set properly, then there are chances that we may get the some errors like this. We may get lobed shafts. Now, if we measure this diameter using a micrometer, that means, 2 point contact method, everywhere it gives same value. So, micrometer measurement will not give us whether there is any lobing or not. If it is elliptical shape, it gives the difference we can find the max, this is the minimum diameter and maximum diameter. Then, we can find that if there is any difference, we can find that there is low mobility is there. But for 3 lobe, the micrometer measurement will not indicate whether there is any 3 lobe or not. So, we just measure the diameter and we measure the diameter of the hole and then we try to we calculate the type of fit. What happens is, say we have a diameter of hole is say 20 point 0 2 millimeter. This is the diameter of the hole and then we have micrometer measurement gives that the diameter of shaft is say 20 point 0 3 0 millimeter. So, this is the diameter of the shaft obtained by a micrometer. Then, what we can conclude is the diameter of the shaft is greater than the diameter of the hole. So, immediately we say that the type of fit what we are going to get is interference fit. But in actual practice, when we try to insert this 3 lobed shaft into the hole, it will enter. So, how this is possible? See now, if we try to insert this, so this is the center of the hole O 1 and then this is center of the shaft O 2. Now, when both the centers coincide, then the situation will be like this. That means O 2 is coinciding with O 1, then there will be interference. But in actual practice, what happens is, we have this circle with O 1 center and when we try to insert this, now we can see that there is some clearance. So, what happens is, this shaft will move down and then it will enter into the hole. So, situation will be like this and O 2 will be somewhere here. So, actually we get instead of getting the interference fit as per the measurement, we get the clearance fit in actual practice. So, we should be careful in fixing, in getting the fits. That means, mere dimensional measurement of the or the specification of dimensional tolerance for hole and shaft is not enough, we have to specify the geometrical tolerance also. So, what is the amount of error that can be allowed on the straightness or flatness or roundness or cylindicity. So, geometrical tolerance is also very important to get proper type of fit and for proper functioning. So, now we will have a discussion on the geometrical tolerance. Now, you can see here, the straightness of an edge, say we have a line like this. So, we have a line like this, but in actual practice, when we measure, it may be like this. So, it will vary, the points will vary. Of course, this gap will be very small, it will be in terms of few microns. So, now it is very difficult to machine a perfect straight edge. So, we have to allow some tolerance for the straightness and that we can do by specifying, what is the gap between these two lines. Say, it may be some like 0.01 millimeter or 0.02 millimeter like this depending upon the application. So, straightness is also specified on the drawings. So, it is to control straightness of a line or axis or a surface. So, basically it is gap between two parallel straight lines in a plane containing the considered line. That means, the line may be like this and what is the maximum deviation on the straightness that is allowed. So, that is mentioned like 0.01, 0.02, etcetera. So, now the symbol used for specifying the, say we have a cylinder like this and we will be having so many generators and we want the straightness of this should not exceed say 0.03. So, we have to specify like this. So, straightness symbol is a short line and then we have to specify what is the value whether it is 0.01 millimeter or 0.02 millimeter. So, that value this is tolerance value and this is the feature. Straightness this for straightness like this we specify the straightness. Similarly, we can specify the flatness say we have a surface like this. For example, the guide way of lathe or any machine tool and it should be flat it is necessary that it should be straight as well as it should be flat. So, that we can specify using this symbol, flatness symbol like this. So, we have to specify the what is the feature flatness in this case and then we have to give what is the value whether it is 0.02 millimeter or 0.01 millimeter like that. So, this is how we specify the flatness. It is basically to control the surface flatness and it is area between two planes. So, we have two planes here and the surface in question. So, this is the surface in question all there are many high points and low points on the surface. All the high points and low points should be contained within these two planes which are separated by the given tolerance value in this case 0.02 millimeter. Now, similarly we can we specify the roundness what is the roundness that is allowed. It is basically to control circularity error in the plane in which it lays and then how it is specified we use two concentric circles. So, that area between two concentric circles gives us the roundness that means. So, we have a shaft which is necessary that it should be round, but in practice there will be some variations low points and high points will be there. All the low points and low high points on that particular round part should be should lay within these two circles. So, this value is mentioned what is the amount of tolerance that is allowed whether it is 0.01 or 0.02 like that that value is mentioned and we specify the roundness like this we use that symbol and then we give the value. So, this is how we specify the roundness. Now, we will move to the perpendicularity sometimes it is necessary that the two lines or two axes or two surfaces should be perpendicular to each other. There will be a datum surface and then there will be a working surface. So, that angle between this working surface and this datum surface should be 90 degree. So, that is known as a perpendicularity. Now, how it is specified say we have an angle plate like this and this is the datum surface. So, it is shown like this say A surface A. So, this is the datum and then we have to specify the tolerance for the perpendicularity. So, what we do is we draw a line parallel to this surface and then we mention what is the amount of perpendicularity error that is allowed. So, for example, 0.01 millimetre that means any point on this particular surface should lay within these two planes the surface can be like this or it can be like this or it can be some rough surface like this all points should lay within these two parallel lines. So, the high points low points can be like this with reference to this A and then cylindicity is also important. Now, say we have the symbol for cylindicity is circle with two parallel lines. So, this cylindicity is to be controlled in many engineering applications. So, this symbol is used to control roundness, straightness and parallelism of the cylinder it is a annular space between two coaxial cylinders. So, annular space between two coaxial cylinder we have two cylinders and separated by some distance this is the tolerance value may be 0.01 millimetre or 0.02 millimetre something like that. Now, all the points high points and low points on the complete surface of the cylinder should lay within these two circles and the shape can be like this may be a taper or it may be taper in the other direction or it can be some bell shaped double bell shaped or it can be drum shaped any shape within all the variation should be within this low ball tolerance. Now, how this is specified we have a cylinder like this and then we mention what is the feature in this case it is cylindicity and then we mention what is the value in millimetre. So, this is how we specify the cylindicity that means you take any generator or any circle all the values all the high points and low points should lay within this range and then we have profile of a line say we have our piece like this and then we have a profile like this some radius is there. So, now we have to control this profile variations for that we have to draw we use this symbol the meaning is there will be two arcs parallel to each other parallel arcs separated by some distance and then what is the tolerance is given that means all the lines on the profile on the high points and low points on the profile should lay within these two arcs separated by the tolerance amount in mm. So, that is profile of a line similarly the angularity sometimes we have to maintain the angle between two surfaces or two lines axis and angle is other than 90 degree. If it is 90 degree then we say it is perpendicularity other than 90 we say angularity. So, say we have a part like this and then this is the working surface this angle is to be controlled with reference to this datum surface. So, what we do we draw another line parallel to this and then all the high points and the low points on this particular surface should lay within this tolerance that is allowed it can be 0.01 or 0. depending upon application we can specify what is the deviation from angularity and similarly we have the symbol for parallelism. So, we have a work piece like this and work piece like this and then this top surface should be parallel to this datum. Datum is shown like this. So, this is the datum say A surface is datum and all the points on this particular surface or line should lay within these two lines which are separated arcs are separated by the given amount of tolerance. For example, 0.01 mm high points and low points all should lay within these two lines or two planes. Now, how this is designated? So, it is shown like this we have to use the parallelism symbol and then we have to give the value what is the tolerance that is allowed and then we have to specify datum with reference to which plane this should be parallel. So, that reference or datum surface also we have to specify and then we have another feature concentricity say we have two steps diameter steps like as shown here and then the axis of this particular part should be concentric with the axis of the other part. So, and if there is any deviation then what is the amount of deviation that is indicated by using two circles concentric circles and that is specified like this. So, we have this is the reference datum say this is A surface A and then this axis should be parallel to this or concentric with this within the certain tolerance. So, we specify like this this is the symbol feature symbol for concentricity and then we have to specify what is the tolerance and then we have to specify with reference to which reference or datum like this we specify the concentricity and then similarly profile of a surface sometimes we need to control the profile of a surface. So, in that case what we do is we use this particular symbol the meaning of this is the we have two surfaces like this separated by the given tolerance amount for example, 0.01 millimeter all the points on the profile surface should be within these two surfaces separated by the given amount of tolerance. So, now how to specify the profile tolerance is shown here we have to use this symbol and then we have to mention what is the deviation that is allowed. Now, in this lecture we discussed about the various aspects like selection of fits calculation of tolerance unit value and then what are the factors favoring loose tolerances and tight tolerances we also discussed about the various geometrical tolerances for geometrical features. In the next class we will be discussing about the various positional tolerances how to specify positional tolerance and then we will also say some numerical problems.