【转帖】casting draft and machining specifi

yang686526

casting draft and machining specification
i have a drawing of a part that defines its final geometry. this part is a casting and the current vendor both casts and machines the part. some areas of the final part remain as cast.
any suggestions for a concise note:
i need to say that draft angle is acceptable for casting purposes as long as it does not affect the machined part outcome.
there is a current note on the dwg that states "1 deg draft each side of datum line c unless otherwise specified". on one side of datum line c is a surface that remains as cast. the other side of datum line c contains features such as o-ring grooves, threads, and several other features. the concern is that the draft angle is influencing these features.
any help is appreciated.
typically it depends on the casting process, die cast, sand cast or investment cast which will determine what tolerances are needed.
some of our drawings have a note that say dimensions marked "1" increase with draft and dimensions marked "2" decrease with draft. (there is a triangle around the number.)
i think it is a confusing way to do things, even more so if there is more than one way to make a parting line. most of the other drawings call  out the maximum draft angle.
how are you identifying cast and machined surfaces? we put a finish symbol on machined surfaces and specify the amount of machining stock to be added. all other surfaces are assumed to be as cast.
boldfish,
   i would systematically generate a separate drawing for the casting.  the machining drawing would call up the casting as the material.  this gives you all sorts of flexibility, including the possibility of generating a second machining drawing that uses the same casting.
   let's leverage those tooling investments!
   you can draw/model the acceptable draft angle and call it up on the drawing.
   you can apply a profile tolerance sloppy enough to allow a draft angle.
   i would not apply a draft angle note unless it was absolutely clear where the drafts would go.
                       jhg
   
boldfish,
our company used to approach two drawings for separating casting and machining as drawoh described.
the note of casting used to be as(for your information):
draft adds mass.
unless otherwise specified, the profile tolerance applies:
for dimensions up to and including x.00inch, .00x a b c
for each additional inch, add .0x to the profile tolerance.
best regards!
oliver
boldfish,

missed a row as unless otherwise specified, draft angle to be x degree.
best regards!
oliver
oliverking,
drafts do indeed add mass but we still don't know the process.  investment cast you can get away with less than 1 degree of draft but i wouldn't try that in die cast or perminant mold casting.  i agree with the two drawing approach it eliminates any misinterpretation plus the minimizes the amount of people seeing the finished dimensions and tolerances.  i've run across some casting/machine drawings done by an aerospace company in tempe arizona and they are done right cluttered.
one nice thing about making two drawings is that if you are making solid models (like solidworks), you can take the casting model and add all the machining cuts to it. you will find out pretty soon if there is any problem. making the drawings is the easy part if the models are created.
this process will reduce the amount of time a checker has to spend on it- you have already done the checking, at least the most important of it.
two models and two drawings are our standard too.
we rarely make completely dimensioned drawings for the castings anymore. we use "xx.xxx +dft" or "xx.xxx -dft" to note inspection dimensions on drawing that are expected to be drafted. general notes like "3d file controls all geometric shapes and dimension unless noted" and "typical draft: 2°" lets us change angle as desired. we do have to add geometric tolerances to casting as you can get parts warped beyond imagination from some poor process control.
anything that is machined is then dimensioned from features in the casting not surfaces that may be drafted. (or lines symmetric to cast features in some cases.)
i am still trying to decide whether to add draft and every fillet and rounded corner to the casting model. with some features, by the time you add all these it is hard to find a real point to dimension to. right now i leave off the draft and just add the fillets and corners where it is obvious or where they would be needed whether cast or not. i let the notes take care of the rest. however, i reserve the right to get smarter and change my mind later.
engjw,
   i would advise modelling the draft and fillets.  you can still get the dimensions that you want by showing the sketch that was used to create the feature you are dimensionsing in the drawing.  in the drawing, you just show the sketch and dimension to the sketch lines.  another approach if you are looking a section view, is to create virutal sharps (where the two lines would come together if a fillet was not shown) and then dimension itmes from the virtual sharp.  i use solidworks, but i would imagine that most mcad packages would easily handle this as well.  i also advocate the 2 drawing approach.  its much cleaner and allows for the process to be split up if necessary, for example if a foundry no longer machined the part but still cast the part.  with notes on draft... it would be wise to define what kind of draft you are referring to.  we have a note on our drawings that states that draft is additive unless otherwise specififed.  we then define additive draft as adding more mass to the cast part(not the pattern).  a separate note for "deductive draft where shown" is used to indicate which surfaces have deductive draft.  my personal preference is to model the casting as exactly how you want it to be (fillets and draft) and show it that way on the drawing.  further re-inforce this by applying the correct notes to the dimensions that define those surfaces.  i think this leaves the least amount of possibility that the drawing can be mis-understood.  another recommendation is that you create your machined part model in a separate file from the casting.  the casting can be inserted as a base part into the machined part file, and then you just begin removing material.  this makes for a clean separation and makes data management more straightforward.  i also really like to utilize a geometry compare tool between the cast part and the finished machined part.  i get a great look at how much material is coming off the cast part and can verify that enough meat is on the casting to always leave a possibilty of cleaning up.  the manufactruing guys really like to see this kind of information as well.
pete yodis