We usually do one drawing per part or assembly.
We will tabulate similar parts per only per program or product.
We made a small block with "Annotation notes" linked to part properties like name, description, material, remarks etc...with format text and colors. This can be saved in your design library folder.
Once you pull this and put in any view, it will propogate the part properties and fill-in all details
Hope this helps
All my drawings are 8-1/2" x 11", and I typically place several drawing views per sheet. I don't know that it conforms to any standard or accepted "best practice", but it works for me.
Instead of a BOM, like you described, I use a Note that's linked to the Part Properties. I place it on one view, then copy and paste it to other views (where it will update to the properties of that model), so I only have to set it up once. And on frequently used notes I have them saved as Styles in my Drawing Templates.
To each his own. But I would say that putting multiple parts on one drawing format is a bit unorthodox.
Sometimes, I would create small assemblies as one part, multibody that is, using something like the weldments feature. Then each body of this pseudo-assembly would be represented by the SAME part number but a DASH would differentiate the parts. Then it could all go on one drawing with multiple DETAILS.
This thing above was a quickie, it is a machined plate (green) with a weldment (orange) attached to it with bolts (not shown). The two items slide with respect to each other, so in reality they should be two different part numbers.
This would be like five part drawings with one assembly drawing for a total of six drawings.
Using weldments, this would be two weldment drawings and one assembly drawing for three drawings.
Cheating a bit reduced this to one drawing. For a production part I wouldn't have cheated, but for a one-time thing such as a fixture or jig, no lost sleep.
We usually make one drawing per part. We also have tabulated drawings for pins and washers that use a design table to define dimensions.
When it comes to making drawings always remember that the person who uses the drawing has the final word, not the person who makes the drawing. You are communicating your ideas to someone you may never meet. They should be clear to the person who has to make the parts.
I have actually done both ways, it really depends on how complicated a parts is. A plate with one or two holes in it, just need the overall dimensions of the plate and the hole location and I can fit 12 of those on a single sheet if need be. But a fully machined part with several features that need to be dimensions, yeah one part per sheet.
And when you need notes on the different parts with BOM or custom property information on them in those views, well first make sure that info is in the part as a custom property. That way if/when that value changes (like from a BOM), that value is kept with the part, not in 2 or more places on the drawing, or even in multiple drawings
Then when you make a note and place it inside that drawing view, you can tie it to the custom properties in that view by starting a note, going into the note properties, and hitting the red circled tool;
Then use the setting shown here;
---Once you have a note with the 'Current Drawing View' properties inside it, you can just copy and paste that same note into several drawing views. Each copies will use the values from their view's custom properties.
OR you place the note off any drawing views, then specify the part you want it tied to, with these settings;
--You can select the 'Selection' field and choose a single part in any of the drawing views already on the drawing. However this one will not change value as you copy and paste it.
In summary, have a good idea where the values for what you want are kept; part, assembly, or drawing. And where they might be changed from. Once that is sure, you can link and modify them from anywhere.
The real answer depends on several things.
1. How complex are the parts?
2. Can you easily and clearly convey the details of multiple parts on a single sheet?
3. How will you handle revisions?
4. Is there a company/customer requirement?
For all the companies I have been involved in we did one part per sheet unless it was a tabulated drawing. For in-house use (design and fabrication under the same roof) you can get by with a lot less formality. But if you are sending your parts out for fabrication or assembly or they can vary one from the other in their revision levels then it is so much safer to just keep one part per sheet.
Always one part per sheet(s) for revision control
You might say well.. you can control revision with several parts per sheet(s) but no, it's a rule here where I work and all must be followed !
Following up: We are doing one part per sheet.
Where I work now and in all previous jobs, we have assigned a distinct part number to each unique part and each one gets its own drawing. The drawing file name and part file name are the same with the appropriate extensions.
Weldments: Individual components of the weldment are drawn on separate views of the same drawing regardless of how many pages it takes.Each component number is the same as the weldment (assembly) number and is given a suffix (dash #) to identify it.
Tabulations of similar parts such as washers and spacers are put on one drawing. The table on the drawing defines the dimensions and perhaps color of each unique part . It can easily be made from the design table.
One part one or more sheets, depending on the complexity of the part...
As others have stated, it really depends upon the end user. Someone else had also mentioned that revision control is easier with one part per sheet. But, even that may not be an issue in many small companies, as long as there isn't a guy with a CNC machine that he pre-programmed for one of the parts.
I will relate a story from a short-term CAD job I had early in my career. I was doing some drafting for a contractor that was doing some work for the military. The policy was for all sheets to be E-sized, and only one part per drawing. So, we had E-size sheets with things like a 12" square plate with 4 holes. I asked why we didn't put multiple parts like that on one sheet. He said the customer wanted one page per part. And then he added, "It also looks impressive when you deliver the drawings using a hand truck. It shows that you did a lot of work".
We typically use ANSI D-size sheets, so we often put multiple parts on a sheet. We just make sure there's enough room so you can differentiate one part from another. We don't really revise parts. If it is just a matter of adding or fixing a dimension, we'll revise the part. On the other hand, if the change affects form, fit or function, we'll roll the part number. We don't want multiple versions of the same part number on the shop floor. That's a sure recipe for trouble.
I just wish SolidWorks would handle multiple assemblies better. The way it is on the indented bills, each part is listed, with common items listed over and over. That makes the bill far bigger than it needs to be. NX does bills with multiple assy's so much easier. Solidworks needs to step up their game. Just my $.02, YMMV.
Most of us at my company do 1 part per sheet. We have 1 person who doesn't conform to the rest of us and puts 2 or more parts on one sheet that are either very similar or are used in the same area of the assembly - it drives everyone nuts . We also only use 8.5 x 11 sheets.
The problems come in where he does not clearly differentiate the parts by number. The sheet has a part number but there are 2 or 3 parts on the sheet - what is the number of each????
He will submit the drawings for machining and say he want 3 - is that 1 of each or 3 of each or one of that and 2 of that and non of that one. We don't know. Usually he will identify the quantity of each or cross one or more out. However, Our database gets the order placed as 3 pcs. of the part number of the drawing - but we don't really know (looking at the database) which one (or ones) were actually made or how many of each.
Then what is the machinist to enter as the program name - they have to create their own reference and the next time we need one of these parts they can't find the CNC's files for that part so they recreate it almost every time.
It gets very confusing, the quantity tracking is impossible (looking back at the database to see how many were made), the machinists re-do the programming work every time (mistakes can happen or parts may be different on different runs due to errors), wasted time and money.
It's so much less trouble to just have 1 part on a page.
Well said Rick McDonald
For me the deciding factors are...
- Finding the Part
- Finding the Part
- Finding the Part
(Let's say that a part breaks and you need a replacement, having it buried in a multiple part drawing or filing it some dumb place, now whoever needs too find the info will thank you dearly for burying it)
Its' not about saving paper, its' about filing it so someone can find it long after your gone.
FWIW, when we do more than one part on a sheet, there is a "BOM" under each part with part no, desc, and QTY. Also for example if 3172-205 and 3172-206 are on the same sheet, then the tab at the bottom of the drawing will have 205 206 on it.
But for this one customer, it's one part per sheet.
Once you get used to it Multiple Tab Drawing file with one part per sheet, you won't want to go back. There is more work inserting multiple parts in one page then it is single part single page, unless you have your drawing templates setup with pre-views etc, but you have to add a BOM where all that should be captured in the title block.
Having said all that, I do want to qualify that I don't have a problem how you decide to do it and it's no hair off my knuckles if you don't do SW like I do - it took me a long time getting where I'm at now and over the years it was fine tune this and then scrap it and start over, now I finally have a system that works well every time for every project and when I see someone else doing it like I did before and knowing the difference now, I can't just sit back and say nothing and let people just slog along, there is a better way, a quicker way, but it might not work for your internal system..
Rick McDonald wrote:
. We have 1 person who doesn't conform to the rest of us...
...it drives everyone nuts...
...wasted time and money...
Is this the owners kid or does he have incriminating pictures?
It' not who you know it's who you ......
Rick Becker He has some leverage because he was instrumental in the early days of the company for making the company a success. He is a good and fast prototype equipment designer that can also do the software and firmware required and was one of the key employees when the company was started. He is highly regarded in his design abilities in that way (by me as well).
However, he is very set in his style and methods and adamantly wants to do things his way. He is the one person here who still uses Inventor and we all have to convert his designs to SWX for manufacturing and support.
He also designs for "building systems from the ground up" and so rarely has to repair or especially do field repairs that he doesn't consider the repair or service side in the design (my pet peeve with him). The designs are also not conducive for efficient manufacturing of multiple units.
I had to do an installation and training trip to a company where we shipped a system he designed and assembled. In shipping and assembly shifted because he did not tighten a couple mounting screws firmly. Those screws were not accessible and are key mounting screws that held the alignment of the key structure. I got lucky and had some special shortened wrenches and it only took about an hour to get to the screws, tighten them and then reassemble the system (all with the customer watching in a high grade clean room - hot - face masks and shields, full coverage smocks (semiconductor manufacturer)). Besides the embarrassment and that it was a first item to this large customer for evaluation, these critical screws should have been designed for easy access and secure locking down. That is just one example of many.
Because of these type things - he does most prototype work and the the designs are passed out and the rest of us do "manufacturing" side of the products. We modify the designs when needed and do the service, training and repairs. It works, just not as smooth and efficient as we would like. I am currently converting one of those tools to SWX and have taken over the project (as is typical).
In successful companies you need the "Natural Disaster Person", constantly followed by the "Red Cross"
If I have a multi body part then one drawing with multiple sheets but most of what we do here is one part - one drawing. Just makes it simpler, IMHO and we use a PDM system so that keeps all things together as they should be.,
For the most part we do one part per sheet . We will do multiple parts per sheet when detailing parts for an assembly that all go together just to save paper, but these are not sent outside the company.
For multi part sheets I have a dynamic note saved in the library that you can just drop onto a view with the part number, description, material, and quantity.
One part per sheet. Sometimes a Part is an assembly. But each of the parts to make that assembly will have a sheet. We have some old AutoCAD Drawings that are like items and are on a tabulated drawing. But when we convert to solid works they all get their own sheet.