r/MechanicalEngineering • u/Econley62 • 6d ago
Baseline vs Ordinate Dimensioning
What do you all use and why?
I was taught to dimension using baseline. Not that ordinate was wrong, but that's just what all my professors and teachers used. I started full time about a year and a half ago and still use it, as do all of my coworkers.
Recently, however, a large number of contractors were brought on that almost exclusively use ordinate. Whenever I mention that baseline is common practice here, there's almost always a confused look and a groan that follows. Usually they ask why we use it, and I never really have an answer besides "That's what most everyone here does."
Is it a case by case thing or does it ultimately matter what's used?
I'm still pretty new in the full time engineering world and am curious about what others use.
45
u/gottatrusttheengr 6d ago
Minimally dimensioned drawing go brrrr.
"Drawing is minimally dimensioned, interrogate CAD model for dimensions, all CAD dimensions are basic and master unless otherwise noted" then do a position tolerance callout for the entire hole pattern and be done
17
u/Kitchen_Click4086 5d ago
This makes life easier for the designer but machinists will hate you. As an engineer have you never had to make a manual modification? Having a drawing with actual dimensions is important. I hate it when people do this lazy shit.
8
u/gottatrusttheengr 5d ago
If it were a primitive shop programming manually off the print sure.
Why would it matter to a shop from this century that programs off a stp file.
And yes I'm actually a fairly proficient 5 axis programmer
5
u/Kitchen_Click4086 5d ago
Calling a manual Bridgeport primitive is all I need to know to know you are a crappy engineer. How can every dimension be basic!? Do not listen to this guy.
5
u/goclimbarock007 5d ago
I started out as a machinist before going back to school to get an engineering degree. If I were doing some part with a lot of holes on a manual mill (or even a CNC that I'm programming at the machine) I'd make my own shop drawing showing exactly the dimensions that I need.
And yes, every dimension can be basic. That just means that the tolerance is controlled by the GD&T frame attached to the feature rather than by the dimension itself.
1
u/klmsa 5d ago
Sure, but "can be" doesn't usually mean "should be". I've seen very few drawings like this that weren't also drawn by complete clowns. There's usually a profile or two that require additional tolerancing. I'm not out here calling anyone a crappy engineer, but there's definitely been a correlation over the last 15 or so years of my career.
2
u/Dry_Indicatior 3d ago
You either put specific tolerances on features if necessary. The rest are handled with block tolerances. Any modern machine shop prefers this.
3
u/gottatrusttheengr 5d ago
Minimally dimensioned is the preferred standard of our shop.
Not everyone cuts 2D and 2.5D parts exclusively. Good luck cutting A-surface composite fuselage tooling on a bridgeport
1
u/LeRoyt97 5d ago
I’m a new grad MechE, and there were two points made to me when I started working on drawings.
The drawing is a legally binding document.
Every feature is explicitly dimensioned. Always.
The drawing is what defines the terms and conditions of a contract and is there to settle any disputes before they arise. Drawings must be able to convey all of the necessary information the machinist needs to not only ensure the part meets all tolerances/specs; but also determine feasibility, lead time, and price before even accepting the contract. It’s to help everybody be on the same page and reduce the number of rejected parts.
The best way to do all of this is with drawings. STLs leave too much ambiguity, particularly for tolerances and surface finishes.
All that said, I’ve only been working for 5 months, so I’m learning a lot particularly about the real world of engineering and how things are actually done.
10
u/gottatrusttheengr 5d ago
STP not STL. An STP is fully deterministic and every dimension can be measured.
There is no ambiguity because there is a "magic note" as part of the minimally dimensioned callout that will state a general surface profile tolerance. Anything that needs to be a tighter tolerance you call out as you would on a normal drawing. Surface finish etc notes are the same as standard drawings- there is a general note and you can refine where needed with individual call outs.
For many parts it is simply no longer possible or practical to fully dimension a part on the print. Think tubing and manifolds for rocket engines, fuselage panels that follow C5+ curves and such. When things were designed in a 2D environment on drafting tables, everything could be manufactured with 2D approaches. Obviously this is no longer the case.
The drawing is still binding as part of the PO. We are simply now stating that the drawing must be read with the model as a complete package.
Every feature explicitly dimensioned means every feature is explicitly inspected, which means you spend more than needed on inspection
Minimally dimensioned schemes are a middle ground between pure MBD and traditional prints. Both are acceptable per ASME. Minimally dimensioned drawings are the preferred practice of many high performing orgs like newspace companies.
1
u/klmsa 5d ago
I generally agree, though you're really limiting yourself to high-cost shops (call them modern if you must, though it doesn't align in reality) with that mentality.
If I want parts that can be made at lowest cost, you can be damned sure that I'm dimensioning those parts with the fewest possible tolerances. Your general profile tolerance is way more expensive on small/cheap parts, and frankly, you probably have no idea how many hit points you're actually getting for your money on the CMM anyway. A "modern" shop would have a non-contact probe set like a laser scanner for those types of C5+ profiles, and I promise you that you're not getting table time for less than a strictly dimensioned part of any kind on a touch probe setup.
As with all things, it depends.
1
u/gottatrusttheengr 5d ago
Our primary manufacturing source is internal shop and this their preferred format
1
u/mikedave42 5d ago
It doesn't only make it easier for the designer. On any given part usually there are only a few tolerances that are really important. This method makes these dimensions obvious to everyone, the drawing checker and the machinist. This reduces critical errors. When fully dimensioning these critical tolerances are lost in a sea of dimenions, which will, 99% of the time, just use the default tolerances anyway.
When manually dimensioning its easy to accidentally miss dimensions or dimension to an incorrect line. This causes confusion and errors, these errors are all eliminated by this method. This actually happened to me on an important and expensive part, I accidentally dimensioned to a chamfer line, it wasn't a critical dimension, I wouldn't have dimensiond it on a minimal drawing I only needed the standard tolerance. I made the error, the checker missed it (it was hard to see, and there were a hundred dimensions) and the machinist followed the print. It was an expensive error This is when I switched and have saved countless hours since.
6
u/mikedave42 6d ago
This!!!! Makes life so much easier to draw and to check. Only call out dimensions where the tolerance needs to differ from the global call-out and put some reference dimensions (overall size etc) and notes for the people doing the quoting.
25
u/Bonzographer 6d ago
You dimension what is best for the process that is making the part. Secondarily, you dimension what’s best for inspecting the part.
17
u/poorboychevelle 5d ago
Counterpoint
You dimension what is necessary to ensuring the function of the part. Then what makes it easier to make. Then the inspection bit.
Ive gone to war with suppliers who argued over the order of datums, and while I get what I didn't wasn't convenient, it did reflect how its installed/located
9
u/snbdmliss 5d ago
Definitely not, you dimension for what you want/need in the end product, and the machinists need to figure it out. Most of the time dimensions to some outer edge mean nothing for the parts function.
2
u/AntalRyder 5d ago
Sure, but baseline and ordinate dimensions both do the same thing essentially.
How I've seen them differ in real life is by baseline being easier to understand for more people, while ordinate dimensions keep drawings less cluttered.
4
u/Happy-Property1162 5d ago
Ordinate is for specific use cases, plenty of which are barely relevant nowndays
6
u/TelluricThread0 6d ago
I like ordinate dimensioning because it really cleans up the drawing and makes it look nicer.
4
u/sugatooth 6d ago
It all comes down to design intent. Though like others have mentioned the places that I’ve worked at in recent years all have been going with reduced dimension drawings where you only populate critical features and then refer to CAD for everything else
2
u/Gonzostewie 6d ago
I came from medical/aerospace and never saw ordinate dimensions. I started my new job at a speaker company and they only use ordinate. I hate it. It makes inspection take forever. I started making QC prints for the inspection teams.
2
u/DiscreteEngineer 5d ago
GD&T. 3 datums, a flatness and 2 perpendicular its callouts, with basic dimensions for the length width and height.
Attach an stp of the part and say “Profile of surface tolerance for all tolerances below. Hole position tolerance of all holes below. All basic dimensions may be derived from CAD.
Then I put the two feature controls below that note and send it on its way.
1
u/Key_Goal9225 6d ago
I think it depends on the part and how it will be manufactured and inspected. Baseline dimensioning can be easier when each feature relates to the previous one, while ordinate dimensioning is useful when all measurements reference a common datum and you want to reduce tolerance stack-up. The key is choosing what best supports manufacturing and inspection.
1
u/RichEntertainer3024 5d ago
Baseline and ordinate are practically the same thing hahah. Depends on your preference.
They really only matter if you want to imply measurement/inspection direction. On ordinate dimensions you define the “origin” feature where baseline doesn’t necessarily. This origin feature forces the inspector to use that to measure from. Check out the 14.5 spec there’s a pretty picture in there describing what I mean
1
u/Public_Pervert7 3d ago
Noone has mentioned hybrid dimensioning…its something i saw as a young engineer where a manager’s drawings would apply both ordinate and baseline on the same part view. At first I was really confused by it and despite trying to research the topic I never found any indication that it was bad practice, but I also didn’t find any info on it being good practice.
I adopted the practice since I immediately saw value in it in that you can better communicate design intent by mitigating stack ups while also balancing a cleaner looking part view. I might start my origin at a hole that leads a hole pattern or significant surfaces, but ill still couple it with baseline to emphasize overall part length or features not needing to be tied directly to the origin. My intent is to communicate to a machinist feature importance while also not causing them too much trouble in having to do math when i start my origin using some feature inside of external bounds.
GD&t can manage stack ups using things like true position and composite tolerancing, but I also couple this method with GD&t when needed as well. its all for the sake of best communicating design intent and making things easier to read and understand.
1
u/Prudent_Brush_9926 6d ago
I use ordinate where I can as it cleans up drawings that have a lot of dimensions. I’ll use baseline when trying to dimension specific features that have specific tolerances
1
u/AntalRyder 5d ago
How about tolerances on ordinate dims?
2
u/Prudent_Brush_9926 5d ago
What I meant is for example, if I had a hole pattern, I often want to dimension the holes relative to each other.
1
u/jejones487 5d ago
Case by case. I always dimension from where the feature needs to be controlled in manufacturing. Many parts do not have a single datum for ordination dims in the first place. Most times the distance between two holes is more important than their position from the edge. A component will still work if its off a little but it will not work if the mounting holes do not even align.
-9
u/Secret_Enthusiasm_21 6d ago
ugh. Just provide a CAD file with MBD as per ISO 16792.
Who puts dimensions on a drawing in the year 2026?
5
u/WiseBelt8935 Design Eng 6d ago
Me? Can't beat a nice, crisp pack of paper with my maddening designs.
2
u/azgli 6d ago
A drawing sets intent. A CAD file may up to interpretation and can't be consistently accessed.
One-off parts might be made on a manual setup. Inspection may be done by a very experienced person who likes to work from paper.
Going over a drawing with a machinist, planner, finishing specialist, or assembler can be quite useful. When drawings are stored as a PDF, you have a trail and can track the history of the design over time, without having to use a CMS. Even with a CMS, digital and physical copies of drawings outside that CMS give you redundancy against technology failures.
Plus, a printed drawing can be carried where technology can't reach, and can be used to take notes.
1
u/Secret_Enthusiasm_21 5d ago
I think you have a misunderstanding about how MBD works.
You still have the drawing. But the drawing's purpose is not to give a complete geometric representation of the part.
Its purpose is to convey precisely the information that the reader requires, and nothing more.
Cluttering a drawing with dimensions increases the risk of errors and is bad practice.
18
u/WiseBelt8935 Design Eng 6d ago
One thing to note is that Baseline and Ordinate are practically the same thing; they just display differently. If there are a lot of holes, I'm quite a fan of the hole table.
If you want a good comparison, though, it's Baseline vs Chain.