【转帖】olerance block angle vs. length vs. rule 1

yang686526

tolerance block angle vs. length vs. rule 1
i have a customer drawing. the part is basically a rectangular block with all edges shown at implied 90 degree angles. all tolerances are defined in the title block and asme y14.5-1994 is referenced in the title block. the width, thickness, and length of the part are dimensioned leaving it to the tolerance block to define the tolerances.
the part is molded and requires draft for mold release. the designer argues that the +/- angular tolerance in the title block accounts for any draft required. there are no notes regarding draft.
here are my problems with this...
1) it is my understanding that the dimension and associated tolerance for the width of the part applies to the entire width of the part (i.e. rule 1 because the width is a feature of size). the designer argues that it applies to the width of the upper surface, not the lower allowing the angular tolerance to allow for draft. the designer's interpretation seems to contradict rule #1 yes?
2) due to the thickness of the part and the title block tolerances the angular tolerance can result in a width that exceeds the dimension and tolerance defined for the width of the part. if i am wrong in point 1 above this is a non-issue but i think this is boooogus due to laziness.
i believe i am right but i must admit the designer is so darn passionate i would like a second opinion.
so i think the real issue at hand is this; does the width tolerance control the entire width or just the upper surface?
i think the answer to this question resolves both of my problems one way or another.
thanks for your help!
hi joebk
i believe the width tolerance to control the whole of the width.
so if the part was 100mm wide and the tol was +/- 0.5mm then one end could be 99.5mm and the other 100.5mm so your draft angle would need to fit inside these dimensions.
assuming i understand your question correctly that is, any chance you could upload a file with this part?
regards
desertfox
if the dim is edge to edge, it is the entire surface...unless noted otherwise.
chris
solidworks/pdmworks 08 3.1
autocad 08; catia v5
going to try to upload dummy image to protect customer & employer but the basic concept is illustrated. i stripped all info except what applies so you might have to refer to my op for some details.
using this example my understanding is that the 1.000 +/- .015" applies to the entire width of the part so draft must be applied to maintain this requirement. the +/- 2 degree angle on the implied 90 degree angles contradicts this due to the thickness (3.000") of the part. i.e. due to the 3" thickness and the +/- 2 degree tolerance on the implied 90's the part can exceed 1.015" in width.
the designer argues that the 1.000" specification only applies to the surface marked as "bottom" so there is no contradiction.
i hope this makes my op a bit clearer.
hi joebk
well if the designers intention is to only apply the tol to the bottom side then it should have been made clearer ie:- dimension the top surface so that you can see that there is an allowance for draft angle or indicate that the dimension only applies to that surface, or show draft angle on the component.
i would ask the designer whether he as delusions of adaquacy on his drawing ability, anyway i agree with your original position.
regards
desertfox
joebk,
   i am very cautious about using ± tolerancs for outlines, primarily because of the lack of control over angles.
   your ± tolerance applies to the entire form.  for each of your three cube dimensions, you measure across the faces.  for me, the worst case is that each "rectangle" can be a parallelogram, canted over at the maximum allowable angle.  
   i used to be under the impression that a rectangle with ± dimensions was interpreted as a nominal perfect rectangle with tolerance zones.  when i took my gd&t course, the instructor corrected me.  the iso system works this way.  for asme y14.5m-1994, read section 2.1.1.2 on implied 90° angles.
   i strongly prefer profile tolerances to control outlines.  if there are no notes defining draft, you can be very creative about applying it.  perhaps you can show your customer some of your cleverer interpretations, and scare him into better gd&t!
               jhg
the .000 +/- .015 in the box confused me for a sec.
the proper way is .xxx +/- .015.
the angle tol is good to indicate, but there is no indication of a draft on the part.
chris
solidworks/pdmworks 08 3.1
autocad 08; catia v5
as already noted by others: as dimensioned, this would be a rectangle with perpendicular walls, over the full faces. the +/-.015 sets the amount of "angle" out of perpendicular.
on an injection molded part, we like to have a minimum of .5 degree draft (more is always better). that would be easy on the 1.000 dim. make the mold to fab a finish dim of 3.010 on one side and 2.990 on the opp side, which provides an in-tolerance part with over .5 degree's draft.
if the draft has to be the other way (along the 3.000 dim), the same process would yield a part in-tolerance, but would have less than .2 degree's draft, not good. normally one would have the mold cavity @ the thin dim for ease of mold manufacture.
we get many parts from customers that are not aware of molded part draft requirements. if a part can be molded with draft and still be with-in tolerance, we explain that to the customer and 99% of the time we can go on and make the mold with-out any drawing revision. if the draft requirements will not allow an in-tolerance part, the drawing has to be revised.
  
does the manufacturing process you are using to make this part allow you to meet the tolerances on the print for the entire surface?  if it is a mold do you cut your molds directly from the 3d model?  (i assume there is a 3d model)  if so i think you have a flatness of .015 to work with.  which side of the part is the functional part in the assembly?  if you make the part to 1.00 on one end and .985 on the other you are still with in tolerance?
i think it is pure being lazy on the designer end of things.  if you need draft have him put in the model.  this goes back to making molds completly from the 3d model per kents thread in this forum on model based dimensioning.  
the tolerance block does not allow for draft angle.  it provides the tolerance when a draft angle is sited.  
the purpose of the drawing is to define the part by capturing and detailing its design intent.  if there is no draft shown on the part, how is the design intent being communicated?
  
matt lorono
cad engineer/ecn analyst
silicon valley, ca
the design intent is that the surface could be perpendicular and or have draft. the dimensions that is on the part is leaving it open to the manufacture to produce that part to its most economic way.  per split lines and what not.  that includes tool design, part costs ect.  the draft angle is built into the tolerance.  the final part if it has draft or not will be accetable if the flatness is within .015.  i do not agree with this if the part needs draft put draft on it and dimension correctly.  not half well you know.