First draft of the drawing for the side plate of our off-season shooter robot. Comments on its readability or completeness are very welcome.
This is our first CADed design that will be going out for manufacturing so any help is appreciated!
Check your drawing settings. They look like they’re on ISO. You want ANSI. Your drawing will immediately become more readable.
You have no title block tolerances. Without them, the shop has no info as to what tolerances you expect them to hold. It also doesn’t matter for this part, but the first/third angle projection callout that is normally in the title box is important. Having the wrong one can completely reverse your design intent and result in the “wrong” part being made, with a non-2D part. Right now your drawing is probably using first angle, because ISO. ANSI uses third angle.
In general I would dimension things with multiple copies (holes, a pattern distance, etc) as “_X” as opposed to writing “each”, or “all bottom holes”. On your radius/angle callouts, the quantity should precede the measurement.
I wouldn’t dimension all the lengths of the flats in the pockets. What I would do is pick an origin (a corner, usually, but the bearing bore in the center of the part could work too) and dimension from there to the flats. That way you have fully defined where the features are located and if desired they can figure out the flat lengths from that info.
Do your best to avoid having dimensions placed on top of the part itself. It’s much cleaner if you can.
You don’t appear to have a material listed
Do you really want slip fits for your bearings? That’s fine if you do, but even with title block tolerances in place you probably want to tolerance those holes directly. Our title block tolerances are +/- .005 for a three place decimal…you definitely would not be happy if you want that to be a nice sliding fit and it comes back at 1.121 or 1.131.
If I were making a drawing for this, I might make 2 sheets to optimize readability. One would have dimensions for all holes/bores and the other would have dimensions for all the pockets and the exterior of the part. This isn’t necessary as long as you can fit everything and still easily figure out what’s going on.
Your pattern of holes on the bottom doesn’t appear to have a dimension locating it vertically.
Your (4) 1/4" clearance holes aren’t located at all.
I’m having a hard time figuring out what’s going on exactly with the dimensions locating the bores (because the ISO format sucks, with all the intersecting lines and stuff), but they should really also be dimensioned from a common origin and not feature to feature.
There’s nothing wrong with having the second view on that sheet, but you could eliminate it if you wanted to, by dimensioning the height of the plate directly and adding a note that it be made from .250 plate.
The dimensions are a mess.
I’d recommend trying to move dimensions outside the border of the part whenever you can. Just doing that will make it far more readable.
If you’re sending this to a sponsor / vendor, consider whether you really need accuracy to the thousandth on ALL of those dimensions. (You don’t.)
Since you’re dimensioning to witnesses, you should show the witness marks to make that clear.
Thanks, that’s a ton of great suggestions. A couple questions:
- What are good title block tolerances? Does the ±.005 you referenced simply specify how accurate lengths should be? I’m guessing holes should be within a thou (1.1245-1.1255)? Angles probably within a degree. Is there a good template or recommended set of tolerances that I could use as reference?
- Would a directly toleranced call out for a press fit bearing look like “1.125 +/- .005”?
Good to know, I don’t know what accuracy I DO need however. If you have answers to the questions I asked Cory above I would be glad to hear them.
Since you’re dimensioning to witnesses, you should show the witness marks to make that clear.
Though I was able to lookup what “dimensioning to witness” means I don’t know what it means to show witness marks.
You’re dimensions are measuring between the the intersection of two lines on one end and the similar intersection at the other end. The point where the lines intersect is the witness. Solidworks has a drawing annotation for marking that witness on the drawing. It’ll make it clearer to whomever is reading the drawing that the dimension measures intersection. Also, for what it’s worth, that’s sometimes not a very useful dimension.
Tolerances will depend on the desired end result, the material, etc. For any sort of decorative feature (lightening holes included), you probably don’t need to go more than two decimal places. The title block tolerance specifies a default tolerance for dimensions that don’t call them out explicitly.
How are you planning on machining this? You may not need to dimension a significant portion of it if a sponsor is just lasering the thing anyway and has tolerance numbers for you.
We sometimes skip drawings for things sent to the local community college to CNC or to a sheet metal shop.
Would ordinate dimensions be good for this part? I usually use the ordinate system for my parts.
The sponsor is using a manual mill with DRO. We’re getting fancy, but not quite that fancy.
I took a second pass and addressed as many comments as I could, uploaded here. Hopefully it is a lot more readable and missing less important info :o
If that’s the case, I would highly recommend removing the odd pockets and try to make things out of right angles instead. Do final countouring with a bandsaw and sander. In my experience, doing rectangular plates and holes is dead easy, but the second you want to do precise angles or curves it’s time to move to CNC.
You also may want to move things to 2 decimal places wherver you don’t need the precision of 3.
EDIT: Especially the odd pocket on the left; that would be extremely time-consuming to do on a manual mill.
I thought about the possibility that a manual mill would be used to make that part, before making my suggestions, but assumed it would be a CNC mill/waterjet/laser. That can change where you’d dimension things from.
Your new drawing looks a lot better. Could probably use some more refinement, but in echo the sentiment that this would be an absolute nightmare to make on a manual mil.
Have you shown the sponsor the general idea of whaf you want done? Or will this drawing be the first time they’ve seen it? The amount of work required to make all the external radii and non orthogonal cuts makes this part virtually impossible to make without expending a MASSIVE amount of time. You’re looking at numerous setups on a rotary table to produce all the internal radially arrayed pockets and the external radii. The angled linear cuts on the two left lightening pockets both require complicated setups to make that a single axis move.
If I was a machinist and got handed this print and was expected to make it, I’d be cursing the engineer that came up with it… And then I’d quit. Any non rectangular features on a part are too much to ask of someone with a manual mill, for FRC purposes. Your sponsor will thank you if you can simplify the part for them.
[edit] second the comment by asid61 to do the external contours on a bandsaw and sander. If you need the weight loss from the internal pockets, you could omit them from the print and print out a 1:1 drawing, glue it to the part after machining, drill some pilot holes in the pockets, and carefully jigsaw them out.
They have the general idea but we haven’t shown them the details yet. I can definitely change the outsides and the pocketing to 90 deg. angles and mess with the odd left pocket, but my real concern is another part that they will be machining. In the full model I posted you can see there are two spines between the plates that provide compresison for the ball. Those have to be curved to a precise radius. Here is the drawing for the spine. Is making something like that on a manual mill out of the question?
Yep. It’d be a long and “interesting” job to mill that curve.
You’re probably going to be better off doing the spines out of a material that can be bent/rolled precisely, taking care of the radius that way, and then drilling the holes.
Or you could rough-cut it with a saw and sand/grind it down, as suggested previously. Use the mill for hole-drilling only (and if it’s just that, there’s a drill press wanting some attention, I’d assume).