This is more of manufacturing question in general.
say I have a shaft of 6mm and I want to have it go through a gear. Should the diameter of the shaft and the diameter of whole in the gear match the shaft diameter? or should I manually introduce a clearance in the gear (or shaft) so that they can fit together?
John, the short answer is yes, you need to compensate for tolerances of the shaft and hole. All machine shops will need a tolerance, depending on the machining used. You could have the shaft ground, at high expense, with tolerances of 0.0005 perhaps. And you could have the hole honed to a tight tolerance, again at some significant expense. So if your going to farm out the parts to a machine shop, you’ll need to design for tolerances.
When designing in shapr, should clearances be in the designed itself? or should this information be noted in the drawings?
I’m thinking that its much easier (in shapr at least), to work in whole-like numbers when building prototypes than to always having to substract + add some clearance between parts — Especially since the clearance could be different depending on the material and/or process that is used in manufacturing.
Or is this process of “fit” a separate process that is done after the design is complete?
Shapr3D are still working on drawing and tolerance updates. I don’t believe we can currently specify non uniform tolerances. i.e.: +0.000 -0.003 for example. If I were to use Shapr3D for tight tolerance design, I would use nominal design, but would allow for one part to be full + tolerance, and the other full - tolerance. This eliminates ambiguity. It’s always best to use the drawing as a reference, and speak with the machinist to red line the drawing, based on the machining methods that will be used. Then I update the drawing with a new revision. I’ve been designing and machining for over 40 years, but I still learn something each time I speak with a machinist about a design.
Currently Shapr 3D doesn’t have any tolerances , correct ?
I have been including tolerance using notes in the drawings. It’s a bit time consuming but it does convey the design and manufacturing intent.
ISO/BS8888 drawing standards state that all CAD items are both master (in the absence of data on a drawing) and should be middle limit on tolerances wherever possible.
I believe this is due to the increasing use of CAD files being loaded directly into CNC machining, wire cutting, laser cutting, 3D printing, etc, machines - unlike the classic approach of manually programming the CNC, or manual milling/turning parts, where dimension and tolerances would be read directly from paper drawings.
This can make it a bit tricky with the classic approach of using ISO standard fits, e.g. H7/h6 hole and shaft fits, which are often based upon a nominal size for both the hole and shaft (e.g. 10mm) but with unequal tolerances on both (e.g. shown on the drawing as: 10mm +0.000mm +0.015mm on the hole, 10mm -0.000mm -0.009mm on the shaft).
(Images from Limits, Fits and Tolerance Calculator (ISO system)
This example should allow both parts to fit together in all cases - from a (relatively!) loose fit with 0.024mm clearance down to a size-for-size fit with 0.000mm clearance (albeit with a bit of effort likely required).
But yes it is good practice where possible to set the tolerance for a face/feature to mid-limit.
In the above example, it would be sensible to change it to be something like 10.008mm with a +/- 0.007mm equal tolerance on the Hole (well it would be 10.0075mm +/- 0.0075mm if being super precise!), and 9.995mm +/- 0.005mm on the Shaft.
As mentioned by molligdj, unfortunately Shapr doesn’t have any way of managing tolerances on drawings/parts yet (which is a must for any meaningful engineering drawings, along with GD&T call-outs for things like roundness, runout and perpendicularity), but I know it’s on the roadmap, and it’s been great seeing the functionality of drawings improve more recently.
To answer the OP question, yes you should (according to ISO standards) update the model to be the nominal, mid-limit size you want the feature to be;
so hole slightly smaller than the shaft if you want to press/push them together, or hole slightly larger than the shaft if you want them to slide together. Also, whatever tolerance you put on the feature should be equally disposed around the nominal size: e.g. 10.005mm -0.015 +0.015mm (or +/- 0.015mm for short).
The actual size of the hole and shaft (or key and keyway, slot, groove, etc) and tolerance will depend on the type of assembly method you want to use, and the function of the part.
You could use a looser, clearance or ‘sliding’ fit if you planned to hold a gear or pulley with a locking nut, bolt or adhesive, but would require an interference or ‘press’ fit if you wanted to rely purely on the fit and friction between the 2 parts. You may even need a heavy interference fit for high torque applications, requiring expanding the pulley/gear using heat (oven or blowtorch), then ‘heat shrinking’ it onto a colder shaft.
Here are some examples of the types of commonly used/recommended fits and how they relate to the ISO standard fit calculator (eg, H7/h6) I linked in the previous post (Limits, Fits and Tolerance Calculator (ISO system)).
As mentioned above, once you’ve found a fit you think is suitable, you’d be wise to translate it to a mid-limit tolerance and apply the nominal size to each relevant feature;
(Taken from Preferred Fits and Tolerances Charts (ISO)