I’m not sure where to put this thread b/c I’m not sure if the drawings I’m talking about are generated in inventor or elsewhere.
My question is about the drawings that are published about the field, giving teams the ability to recreate field elements from accurate drawings. They have the first logo in the bottom right corner and there’s usually a “cover” drawing with a sort of “finished product” then the pages that follow show each component and how it’s constructed, and each page usually has a mini BOM in the corner.
My question is how do I recreate these drawings (from my own assemblies and parts in inventor)? Are they produced in inventor or somewhere else? If they aren’t from inventor is there anyway that I can make them from Inventor (of my own assemblies and parts)?
Right now CAD has little to no place on our team because we have no way to practically use it. If we had the ability to make these drawings we could print them out and actually use them during the building process. It would sure be better than the drafting table and cardboard cutouts we’re using now.
Thank you in advance and sorry for posting in the general forum area. If someone could help place this question better I’d appreciate that just as much as an answer.
To help make drawings like the ones FIRST gives out you would probably have to model the field in inventor and make .idw’s with all the parts.
this should probably go in the CAD section of the forum
also I don’t have any idea where to find the field in CAD but to help CAD become a bigger part of your team, you might want to consider modeling up parts of systems in inventor before you make it. Inventor has a great part analysis program that can help immensely with making sure a part is strong enough to do its job. Even if it is just one thing. also if you model everything in inventor you can have your entire robot in your pocket, that weighs like 2 grams (in a flash drive) which is always helpful.
All right, time for someone with some knowledge to chime in… (Though I’m sure Craig Hickman or roboticWanderor or some of the other experts will show up soon.)
Here’s the general procedure: Go to “New” and select “Drawing”, using your favorite CAD program. Then, import the part/assembly you want (sorry, I don’t remember the path–it’s usually pretty obvious). Now, create more views–they’ll automatically run from the first one.
There may also be an option to create directly from the part. I know Solidworks has this (File->Create Drawing from Part); Inventor might, too, but it’s been a while, so I don’t know/remember where.
As for the block fill-in, I have no idea how to do that so that it’s custom.
And yes, we do have a CAD subforum with specific subforums for three different progams. Any questions on CAD can go there and get a fairly fast response.
I use SolidWorks, so here’s how it goes. (Inventor was a similar process).
Model your robot in CAD. Simple enough, you need parts to make drawings.
Once you are done, go to File > New and make click Drawing.
If you have not created a custom title block yet, just select the default template for the size drawing you want to use. Personally, I do everything on either 8.5"x11" or D-size (24"x36").
Before you put any model views in the drawing, you need to customize the title block. Well, you don’t need to, but its nice having a custom team title block. Right click anywhere on the drawing and go to Edit Sheet Format.
Use the sketch tools to recreate the title block the way you want it. Don’t delete the text-holders from the default template, they will automatically be filled in if you set each model correctly.
When you are completed, go to File > Save Sheet Format. Give it a file name with your team name and the page size. It will now show up in the list of choices when making a new drawing.
Import your part into the drawing. Create multiple drawing views as necessary, and dimension and tolerance as necessary. If you want to make an exploded assembly, you have to open the assembly file, use the Exploded Parts feature, and then use the Exploded Part Sketch feature to add lines in there. Save the file and import into a drawing. Label each of the parts as necessary.
For assemblies, or parts with multiple revisions, it will be helpful to add a revision table and/or list of parts table. SolidWorks automates a lot of this stuff to make it go a lot faster.
Save the drawing. I always save it in native SW format, as well as an additional copy in PDF form. The PDF version is much more convenient to email or print out.
It’s also a really good idea to take a course in drafting or creating engineering drawings. Engineering drawings are a form of communication, so they should be as clear and to the point as possible, containing all necessary information.
If you are serious about doing this in the future, it would also be a good idea to figure out a part naming scheme and give individual part numbers to every component you design. (Calling something “Delrin spacer” or “3/8” Drive Shaft" gets really confusing). Team 228 did this for every fabricated part on our 2009 robot; we filled an entire three ring binder with the part drawings.
Also, if your team is considering seeking the help of an outside machine shop to make some parts for you, having proper drawings for all of the parts REALLY helps the machine shop, and ensures you get back the exact part you were looking for.
You will see how to modify the sheet format and insert your model.
Creating a custom sheet format can say you lots of time when you are making a series of drawings. You can also insert a picture in .jpeg format of your team’s logo into your title block and team name. Once you have your sheet format, you can use it for every drawing.
The title of the drawing will follow the part file name, however this can be modified as a custom property. The more properties you define in the part, the better. For example if you define material in the part, you will automatically get material in the standard SolidWorks title block. You can insert Weight into your titleblock as a custom property. If the part changes, the weight displayed on the drawing will also change. Depending on the units you set this may be Mass and not Weight. The Material will propogate to the Bill of Materials in the assembly drawing.
