Hello everyone, My team is deciding to switch from Bottom-Up to Top-Down CADing method and I’m the one that’s teaching them this new way. I was informed the reasoning behind this change is to improve the speed at which we can CAD at. I was told that in a top-down method you can work inside the assembly which in turn can speed up the process as you do not have to keep getting measurements, making guesses and swapping tabs . There are a few **concerns **i have with this however,
if we have one assembly for the robot only one student can work on it at a
time without erasing the other’s work.
multiple students can’t work on and in the same subAsm/asm. * example (we are making a cube that’s hollowed on the inside. I
then assign 6 students to go create the parts in a topdown method.) is this even possible or would it then be considered bottom
up method, and how would this work with none existing geometry which is the advantage for topdown? *
is this even a good method to use for a robotics application.
I was told about methods used with top down cadding in solidworks called, brake and lock. would these be solutions to my problems, and if so are there any good tutorials for me to watch so i can then teach the students? and my “skill” level if it matters at all for the tutorials.(I’m certified in Solidworks can’t remember the level, and have been using it for about 6 years. I’ve only ever used bottom-up design methods though)
any other advise or info is much appreciated, Thanks.
Our method is to have each sub-assembly working mostly separately. They each have a roughly nightly build of the robot to use but they only save changes to their own sub assembly and parts. Then they push their changes to GrabCAD and the new master assembly updates with the various sub assemblies when ever they pull from GrabCAD. So people can being working in the main assembly (have that open) as long as they remember to push only their sub-assembly or the parts they modified.
This has worked pretty well but there are errors sometimes and a couple times people lost some work cause it was over written in the main assembly and they had to redo some mates but that isn’t too time intensive.
This worked with about 6 people doing the majority of the CAD work and a few other’s contributing parts or making small modifications as the build went along.
While I personally love top-down design, SolidWorks’s handling of external references is very fragile compared to other CAD packages. It’s one of the real weaknesses I’ve found with SolidWorks.
This is pretty much the right approach, I think. I’d add two things. First, you have to make sure somebody is maintaining the master assembly and ensuring that communication is flowing so there aren’t any conflicts. I’m sure Allen’s team does this but I thought it’s important to mention.
Second, I’d say designing the individual subsystems top-down is a pretty good idea. Anything I design is 95% laid out in a single sketch before a single part has been drawn. That way you can get all the geometry out of the way and make sure it’ll work, instead of “getting measurements, making guesses and swapping tabs.” Maybe you can call it middle-out design?
Interestingly enough our entire robot was modeled Top-Down this year. You’ll get a bunch of mixed opinions about it, but I do want to talk a bit about both the good and the bad. Proof: http://i.imgur.com/YzadJJLl.png](http://i.imgur.com/YzadJJL.png)
Good:
Very fast to CAD out entire assemblies
Very easy to adjust dimensions of entire mechanisms as multiple bodies are generated from the same sketch
Having every subassembly visible allows for much more effective packaging
I personally really enjoyed it in the beginning because it was so easy to make the drivebase and integrate the superstructure. Drivebases are typically things where several different elements come together and having everything work together is very helpful. Every rail is connected to a single sketch that defines the robot’s width, length, number of wheels, etc. However I would strongly advise against Top-Down design for your entire robot, at least in Solidworks. Here’s the bad:
You effectively break any sort of revision history. GrabCAD or your pdm will not help you when you ruin the master part and wipe your local drive. Solidworks handles Top-Down through Split Assemblies that are **very **
finicky. A “save-bodies” operation is actually a feature that gets added to the bottom of the feature tree. The save bodies operation relies on a specific body (never merge bodies in features!) to generate. Exporting your master part for assembly (adding wheels, motors, etc) must must must be the last thing you do if you want to save yourself some headache. If you decide you want to combine two bodies into one or split one into two, you effectively broke the “Save Bodies” feature that contains it and every other associated body. - You need very strong part management and everyone who contributes has to export bodies in a very specific way. Every body gets converted into a split part that will all spit out into the parent folder. You need to be careful or you’ll be dealing with tons of parts in the wrong folders.
Do not
put the entire robot in one master part. This was amazing for me to fly through the CAD process, but effectively nobody else on our team could contribute due to differences in skill and my local changes not being pushed to GrabCAD. I alone made over 280 pushes to our GrabCAD throughout the season and what was in the cloud was still not up to date. - Impossible to revisit old ideas. We changed our intake design throughout build season and had already bought a significant amount of parts for the original design. I had to suppress the original design in the master part to save the numbers, but it was risky as each sketch was defined from sketches before it. That said…
ORDER MATTERS! You really need to understand the feature tree to save yourself a few headaches. When defining new subassemblies, I recommend hiding everything so you don’t accidentally click an edge of a body instead of a line in a sketch and ruin everything past that feature. I eventually found the roll-back feature extremely useful in identifying mis-ordered references, but Solidworks simply does not do a good job in this process.
This is just a bit of what I’ve experienced after a season of Top-Down. Honestly I would rather jump into PTC Creo to do Top-Down rather than Solidworks. The best advice I can give you is to make a drivebase top-down and then the master “sketch” on top if it. You can export the master sketch to other master parts and do Top-Down on each subassembly. Some times too much flexibility can hurt you in the long run. YMMV!
