Baixe 08 - Tolerances e outras Notas de estudo em PDF para Engenharia Mecânica, somente na Docsity!
Working With Tolerances
By D Cheshire
Page 1 of 5
Most CAD systems have functionality to allow the user to add toleranceinformation
to^ dimensions.
This^ allows
drawings
to^ reflect
design or
manufacturing intent but since the tolerances are nothing more than anadditional text note applied to the dimension no additional functionality canbe gained from the tolerance value. These ‘unintelligent’ tolerances canserve no benefit for analysing such things as tolerance build up problemsand volume/weight variations.Pro Engineer builds three-dimensional models and allows the definingdimensions to have tolerances applied to them. These tolerances can bedisplayed in the three-dimensional model window as well as appearing onthe subsequent drawing derived from the model. Since these tolerancesare inherent in the defining dimensions of the part they can be used in amuch more ‘intelligent’ way for analysing the parts performance in anassembly as will be shown in the following scenario. Tolerance Overview All Pro Engineer components are built with nominal values. The nominalvalues^ represent
the^ ideal
sizes^ that^ are
intended
by^ the
designer.
However
manufacturing
practice
dictates
that^ no
dimension
can^ be
guaranteed exactly. All manufacturing processes require a dimensionaltolerance range within which the size can be guaranteed. The smaller thetolerance range required the more expensive the manufacturing processrequired is^ likely
to^ be. Assigning
very^ narrow
tolerances
to^ every
dimension causes a component to be more expensive than is necessary toachieve the function intended. It is the designers’ role to analyse theproduct and decide which dimensions are critical to achieving the productfunction.All dimensions entered in Pro Engineer are given a default tolerancevalue.^ To
see^ these
values^
make^ sure
that^ the
option^
DIMENSION
TOLERANCES is checked in the TOOLS >
ENVIRONMENT dialog. Every
dimension for a feature will now be displayed with tolerances shown. Alsothe part window will display the default tolerances as follows…
X.X^
X.XX^
X.XXX^
ANG^
This shows that the default tolerance varies according to the number ofdecimal places assigned to a dimension. The number of decimal places is
determined
whilst^
in^ the^ sketcher
by^ SKETCH
>^ OPTIONS
on^ the
PARAMETERS tab under NUM DIGITS. The default values, shown above,can also be changed choosing ANNOTATION in the selection filter at thebottom of the screen and double clicking on the tolerance value. Anymodifications
you^ make
to^ these
default
tolerances
apply^
only^ to
dimensions
subsequently
created.
Previous
dimensions
will^ have
the
default tolerances active when they were created. If, for example, younormally
work^ with
a^ general
tolerance
of^ +/-^
0.3^ on^
all^ unspecified
dimensions, you could change all of the linear values to 0.3 and thenassign suitable tolerances to individual dimensions as required later. Assigning Tolerances To Part Dimensions The two components shown in Figure 1 and Figure 2 are simple partswhich are intended to fit together as part of an assembly. They are to beconstructed as two separate Pro Engineer parts called tol1 and tol2. Usingyour existing knowledge of Pro Engineer create these two separate partsnow using mmns_part_solid template. The L shaped block in tol1 can becreated as
an extruded
protrusion and the three pegs are a
second
extruded protrusion created by sketching three circles onto the top face. ENSURE YOU DIMENSION THE PARTS EXACTLY AS SHOWN
Figure 1 : An Engineering Component Called
tol
Working With Tolerances
By D Cheshire
Page 2 of 5
Figure 2 : A Second Engineering Component Called
tol
Having created the two parts it would be interesting to see what tolerancehas been applied to each dimension. Open part tol1 now. First make surethat^ the
DIMENSION
TOLERANCES
is^ checked
in^ TOOLS
^ ENVIRONMENT. The default number of decimal places in sketcher is 2.If you have not changed this or the default tolerance values the toleranceon all dimensions with two decimal places X.XX should be reported in thegraphics window as +/- 0.01. Confirm the tolerances are as you expectedby right clicking on a feature in the model tree on the left of the screen andchoosing EDIT. The dimensions should now be shown with their upperand lower limit values as you can see in Figure 3.
Figure 3 : Tolerance Shown
As an example of what tolerances can be used for at a part level thevolume of material in a component could be calculated. Clearly since thedimensions have a tolerance the volume would also have a tolerance. Tofind^ out the^ volume
range^
we^ need
to^ calculate
mass^ properties
at
maximum and minimum material conditions. The part dimensions are setto an extreme value by
EDIT^ >
SETUP
>^ DIM BOUND
>^ SET ALL
UPPER^
>^ DONE.
Notice^
that^ SET
ALL^ can
be^ used
for^ tol
since
maximum material conditions are when all dimensions are at the upperlimit. If the part had a hole the dimensions for the hole feature would needto be set to the lower limit for maximum material. The volume can now becalculated using ANALYSIS
^ MODEL ANALYSIS and choosing the Type
as Model Mass Properties and Compute. The density can be set to 1. Notethe volume is calculated as 76 495 mm
- The calculation can now be
repeated after first setting the dimensions to minimum material conditionusing EDIT
>^ SETUP
>^ DIM BOUND
>^ SET ALL
>^ LOWER
^ DONE. Note
the volume is calculated as 75 863 mm
3 a total variation of 632 mm
- Use
EDIT^ >^ SETUP
>^ DIM BOUND
>^ SET ALL
>^ NOMINAL
^ DONE to reset
the bounds to their normal state.
Figure 4 : Mass Property Calculations
Working With Tolerances
By D Cheshire
Page 4 of 5
Analysing Assemblies with Tolerances The holes
and pins
in^ parts
tol1^ and
tol2^ are intended to
assemble
together with a clearance fit of H9e9 as designated by BS4500. Referenceto^ this^ standard
shows^
that^ the tolerance
for^ a^
12mm^ shaft
of^ this
specification is –0.032 to –0.075. The matching hole would be +0.000 to+0.043. Change the tolerance of these two features now. In the tol1 partright click on the feature for the pins in the model tree and choose EDIT.Since you just set the tolerance mode for the diameter dimension to Limitstwo diameter values (12.01 and 11.99) should be displayed. Double clickon the lower diameter dimension value for the pins (11.99) and type in thenew value of 11.880. Double Click on the upper dimension value (12.01)and type in the new value of 11.950. In tol2 you will need to Edit thefeature^
then^ click
on^ the
diameter
dimension
and^ choose
EDIT^
PROPERTIES so that you can set this to Tolerance Mode Limits. Thenrepeat the changes setting the lower dimension to 12.000 and the upper to12.043.To illustrate these concepts create a new empty assembly called tolassand assemble the two parts, tol1 and tol2, together. Use tol1 as the firstcomponent. Apply three constraints as tol2 is placed as shown in Figure 8.Make sure that the first mate constraint references the end from which the15 dimensions is taken on tol2.
Figure 8 : The Assembly Constraints Once the assembly is complete analysis can take place. One problem thatoften occurs with tolerances is that assembled components will not workcorrectly when the parts in an assembly are all at one extreme of size.ProEngineer can calculate whether two parts in an assembly interfere with
each other. In the assembly tolass issue the command ANALYSIS
MODEL^
ANALYSIS
and^ choose
the^ type
of^ analysis
as^ PAIRS
CLEARANCE. Pick the two parts in the assembly and Compute. At thisstage ProEngineer should report a zero clearance. Of course since the twoparts are designed to touch along two faces this is what you would expect.What is the clearance between the pins and their holes? To find this usethe command ANALYSIS
^ MODEL ANALYSIS and choose the type of
analysis as PAIRS CLEARANCE but this time choose SURFACE as theFrom and To option. Pick on the cylindrical surface of one pin then rightclick^ until
you^ pick
the^ cylindrical
surface
of^ the^
corresponding
hole.
ProEngineer should report a clearance of 0. 0.0529799mm and a redmarker will be displayed at one of the points of minimum clearance. Why isthere this clearance value? Because the calculations are currently beingperformed on the parts at nominal sizes. The calculation is…Pins at (11.88+11.95)/2=11.9150mm diameter.Holes at (12.043+12.000)/2=12.0215mm diameter.Clearance of (12.0215-11.915)/2=0.053mm.If you do not get this value make sure you have set the dimension boundsto nominal (EDIT
>^ SETUP
>^ DIM BOUND
>^ SET ALL
>^ NOMINAL
^ pick
part^ >^ DONE for each part).The question remains that if the parts are at their worst extremes oftolerance will the parts still assemble? What are the worst extremes? Thisclearly occurs when the pins are at there biggest and the holes are atthere smallest. Also if the distance between the pins is at a minimum andthe distance between the holes is a maximum (or vice versa) a worst casescenario exists. To achieve this condition in ProEngineer we need to setup the dimension bounds as we did before but in the assembly. Use EDIT >^ SETUP
>^ DIM BOUND
>^ SET SELECTED
^ LOWER and pick the part
tol1 on one of the pins. The dimensions for this feature will be displayedand you can now pick each spacing dimension in turn (i.e. 15mm, 20mmand 20mm) followed by DONE. These will be displayed in white indicatingthey are set to lower. Now using the similar command set the diameter ofthe pins to the UPPER tolerance. This time the dimension will be displayedin grey indicating an upper tolerance. Repeat this procedure for the holesin tol2 (use right click until you pick on the holes). This time the spacingneeds to be set to UPPER and hole diameters to LOWER.The assembly is now set to one extreme of tolerance. If the interferenceanalysis between the two parts is performed again interference will be
Working With Tolerances
By D Cheshire
Page 5 of 5
reported
the^ red
areas^
where^ the
parts^ overlap^
is^ highlighted.
The
assembly will NOT work as intended with the current tolerances. To makeit work the tolerances on the spacing of the holes could be reduced butthis is likely to increase the cost of the component. Is there an alternative?
Figure 9 : Interference
If you look at the previous interference analysis you can see that theinterference occurs on the last two pins, why? The problem is calledtolerance
stack^ up.^ Consider
Figure^
10 which
shows^
two^ alternative
dimensioning schemes.The two schemes apparently are no different until you consider tolerances.If a tolerance of +/- 0.01 is applied to each dimension what is the overalldistance
to^ the
centre of^ the
right^ most
circle.^
Using^ the
chain-
dimensioning scheme the tolerances are cumulative so the answer is 55+/-^ 0.03.
Using^
the^ baseline
dimensioning
scheme
the^ dimension
is
specifically stated so the tolerances do not add up and the answer is 55+/-^ 0.01.
An^ improvement
in^ accuracy
has^ been
achieved
with^ no
tightening
of^ tolerances
and^ no
extra^
cost.^ In
general
baseline
dimensioning is more accurate and should always be used except whenchain dimensioning better reflects the critical dimensions.
Figure 10 : Alternative Dimensioning Schemes
You may like to return to the parts tol1 and tol2 and EDIT DEFINITION onthe features so that the dimensions for the holes and pins reflect thebaseline scheme. If you perform the analysis again you will find there is nointerference and the assembly will work as intended. Review So what should you have learnt?^ •^
How to define tolerances on part dimensions. • How to show tolerances on drawings. • How to use tolerances for analysis. Any problems with these? Then you should go back through the tutorial –perhaps several times – until you can complete it without any help.
