Hello there, some help please. I'm trying to mate these individual sections to create a whole disk (with a 10mm gap between). I cant seem to get the mates to work. What am I doing wrong?
Thanks in advance
It looked like you needed to add some sort of concentric or coincident mate but this over defined the assembly.
I removed your distance mate and made those two faces parallel and the distance was indeed 10mm. I couldn't tell if your 2 parts were identical, but a circular pattern also seemed to show promise (no mates at all)
The distance mate worked when applied to two vertices,
This sort of thing confuses me, I don't know why it's so strict
Thanks Rob, I managed to use a tangent mate by adding a construction line the same diameter as the disk then mating the outside curved face to it.
Appreciate your time tho!
For this type of mate avoid tangent mates, you only need two for this type of an assembly - pick the part edges at the red line = coincident - pick the other two edges at the blue line = coincident
Or you can select the round face at the blue line and mate = concentric
Lee wants to mate with a 10mm distance between the faces, for my own interest I wonder what would be the best way to mate these together allowing that limit mate to drive everything - ie increase or reduce it
I would definitely use a sketch
Yes of course that makes sense
...you're still right but for sheer stubborness I've done it with 2 planes and a load of symmetry
Looks great but think it's a bit beyond me!
I've never had any formal solidworks training (picked it up as I've gone along) so just the confirmation that using a sketch is a legitimate way of mating an assembly is comforting
What I would do is create a sketch like the one below, bring that into your assembly as a part, which you can exclude from the BOM, then mate each segment to (2) two lines (pointed out with the blue lines) using a coincident mate, this will lock in the part. Changing the dimensions in the sketch will move the components accordingly..
I've had no formal training either, just 3 frustrating years. Probably some training would of saved me a lot of hassle in the long run, but I didn't have the choice back then. I read Matt Lombards Assembly Bible which was excellent. Highly recommended (I should probably read it again)
I think part of the problem is that there are so many ways to achieve the same thing - unless you're working in an environment where others dictate or show the way, if you're a newbie on your own - it is idiosyncratic and confusing. Every different method seems to have distinctive merits and limitations, that often you don't discover until some point in the future. Guess there's no shortcut to experience.
I have no idea if my solution above is any good, it does seem quite complicated but that's why I like to engage with the forum - improve myself, hopefully help others
All the best
Just like John had mentioned, we do the same thing here for gap alignments ... Simply create a sketch to be used at assembly within the part model itself. We even call our sketch out as a "Gap Alignment" sketch and specify the gap distance we expect to keep the design intent clear.
That's right you don't need to save the sketch as a part, it's just that in my workflow I use Sketch Parts all the time and would use it as I mentioned, but your way would work just as well.
Agreed, and to Robs' point I have to admit it's both impressive and frustrating that there really are so many ways to get where we need to be with this software and everyone's individual take on it will most definitely have its benefits and drawbacks alike. If nothing else, I usually learn a different approach to how I would have handled things in the past almost daily. The old adage of "It's the way it's always been done" simply doesn't work with this software, and I like it that way ...
Couldn't have said it better....
This post is a great example of the different ways you can get to the same point at the end of the day, it can also be a huge opportunity to learn new ways, better or worse.. The biggest challenge we're all faced with is "How the company Policies effect what we do", how the shop likes to see the drawings, how management thinks the shop should see the drawings and we need to be the middle man..
Also what does our workflow require, here I get to do "New" designs and the expectation that they have here is multiple changes, and multiple pack & go's so they can see the Chair or Bed side by side, these assemblies must be setup so I can modify it quickly, as simple as opening the Assembly file, clicking on a sketch in my Sketch part, changing the dimension and hitting ok and everything moves to the new size. Or, delete that part and put in another completely different part that is shaped totally different, therefore I need to be sure that when I do delete that part, my feature tree stays intact and maybe a few mating errors from faces that were deleted. There are many times I could do the design a portion of the time, but then it wouldn't be as parametric and easy to change.
So the next guy is faced with different challenges
I'd have made 1 segment then used an array.
Create the overall sketch of the entire assy layout.
create your single segment.
Array around a single axis point.
I'm not sure you have an answer yet or have decided on a practice but if it was me I would create a new assembly file with an Axis suitable for your needs, I might use the Front and Right planes for that, Insert Reference Geometry, you might see the Axis then in the preview. Then I would insert your first part and Mate it to the Axis. You might have to Float that part first to do that. Then just use a circular pattern to add the others using the Axis you created as the center point. I did not open your file.
I put a post on here from my work account.
Seeing however as my comments are moderated I though I'd log in with my old account I've had since Day Dot!
(Couldnt move my old account over when I moved jobs.)
Id have created the initial sketch layout of the overall assembly and then created a single part using a segment of the sketch.
I'd have then array'd the single piece around the center-point of the initial sketch which would have an axis.
Wow lots of amazing comments, and helpful ideas. Great to get an insight into how you folks all work. All these suggestions will keep me busy for a while!
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