CAD drawing for pricing help

[borges1]

Hey all, i regularly produce architectural drawings, but i am trying to teach myself to do drawings for machine work. From great suggestions here i picked up the Giesecke Technical Drawing book and its gotten me pretty far. But now i'm working toward the stage of wanting to have some parts priced by someone who can mill, anodize and potentially laser etch some markings of a portion of my project for small production runs. This is a design for a woodworking tool - if your familiar with Woodpeckers brand tools that is sort of the fit/finish/precision i'm looking for, but that seems to be the common standard now. I'll ask about a good supplier once i am happy with my (seriously homespun) prototypes.

My questions:
1. I am using the full pro version of Sketchup/Layout for my CAD. It is not vector based and has limitations, but i can export .dxf and other formats. Should i just recreate the model in a native format for all the online pricing tools? Or will my model be sufficient along with a .pdf showing tapped holes etc? If redoing the model is recomended any suggestions? Especially coming from the sketchup world?

2. With modern CNC outsourcing what are good tolerances to indicate? Or do these machines produce .000" tolerances over an entire part so baselines are not as critical as an accurate CAD model? Tenths of MM and thousandths of an inch? More or less? There are only a few critical tollerances in my parts, mosty i just want good alignment to a good fit and finish.

3. What is the best way to model holes to get a correctly fitting part, including anodizing? By which i mean, in the model (not .pdf plan) what do i need to include for things like countersinks, sti tapped holes, standard tapped holes, etc? At what dimensionall accuracy in the CAD? I do want an anodized part, and i will add sti inserts and assemble. All tapping could be done after anodizing, but i guess that would be left to the suppliers expertise. Or i could do it once i had the parts, but i've read tapping anodizing is hard on taps.

4. Metric and Standard. Because i can get standard sized aluminum easily, that is what all my parts and models are based on. But all the fasteners are metric since i intend this tool to be primarily used on metric machines so i am maintaining that standard for all the fasteners. Is this a big issue? I cant imagine it is with he CNC world now, but want to check. Should converted dimensions be tolleranced more? Like the scale mounting holes i show on the plan in both units.

5. i don't quite get how to define overall edge finishing. As in its nice to have small chamfers on all the holes, the part edges, etc. This is a tool that is not held, but handled, so super sharp edgees are not desired, but drawing in tiny chamfers, or heavy de-burrs seems silly, and there musts be a 'standard' that all these types of parts are getting. Two examples: for the outside corners on all 4 parts on the plan it would be nice to have a pretty hefty chamver, say .125". On the other edges just some sort of heavy deburr would be appropriate. How do indicate this detail?

Here is the most relevant page from my current working plans. This page shows the 4 most complexparts. I can turn the x-ray view on and off, but i find the interior details helpful while working and this rendering is more clear to me than the 'standard' interior views, dashed lines, etc. yes, i know i need to change the dimesions font

 

[RJSakowski]

In my last ten years as a professional, I had to produce many drawings for outside manufacturing. Here is my take on it. The primary responsibility of the designer/draftsman is to unambiguously communicate the design specifications to make the desired part. To that end, all dimensions, tolerances, a finish needs to be specified. A 3D model can be useful to the manufacture but it must be true to the design; no approximations. Even so, 2D drawings should accompany the model as you cant convey tolerances or finish with just the model.

2D drawings should have all dimensions given once and only once. An example is a linear array of holes . You can give the inter hole spacing along with its tolerance but you shouldn't also give the total distance between end holes. My preference for dimensioning an array of features is to use ordinate dimensioning which gives to coordinates for each hole. Tolerance can be given with box tolerances which give the default tolerance for any dimension unless specifically overridden on the drawing. Be practical in your tolerancing. Tightening up on tolerance means additional cost. OTOH, tolerance are what the manufacturer is going to hold you to if the part doesn't function properly. Remember, your CAD work is your contract.

I had the privilege of working with an excellent CNC job shop. The owner told me up front that they would guarantee +/- .002". However, every part they ever made for us held our tighter tolerance. I believe that CNC machining can easily hold+/- .001" or better nowadays. Whenever I took new CAD work to him, I would take the time to explain what it was that I was trying to accomplish. This saved my butt more than once when he would point out something that I overlooked.

Regarding anodizing or other secondary operations, when I first started making drawings for job shops, I was told by an experienced draftsman that it is the responsibility of the manufacture to account for these processes when meeting tolerances. I had the occasion to design a part which required anodizing and the tapped holes were partially anodized in the process, requiring chasing with a tap for the to function. The job shop should have accounted for the anodizing and either used an oversized tap or plugged the holes prior to anodizing. However, you do have to state on your drawing which surfaces are to be anodized.

As to dimensioning. pick metric or pick inch. If you do want to mix dimensions, use dual dimensioning. I see that you are using GD&T already. This is an excellent way to specify conditions that would otherwise be difficult to convey. For instructions that difficult to convey otherwise, drawing notes will cover those. A note specifying "break all edges" would cover your sharp edges, e.g. Check your drawing prior to release , mentally going through the manufacturing process. If you find a point at which you can't proceed without additional information,you can add it.