Smart Fasteners are Dumb Fasteners

[guru_florida]

Or maybe I'm dumb...ok...but I created a bracket part with some 1/4" socket head holes using the hole wizard. I need a right sided part too, so I selected the right plane and used "Insert | Mirror Part... " trick. Handy, my right side part maintains dependancy on the left, I like it. But then, in my assembly I cannot use the Smart Fasteners on the mirror part as its only a "Solid Model" and it doesnt recognize the hole features.

So, instead, Instead create the mirror part and break references, it creates a copy of the part, adds a "move/copy mirror" op to the feature stack. I lose my dependancy now, but oh well. I can add Smart Fasteners now, but it instead mates the bolts on the opposite side of the bracket. The top head of the bolt is mated to the backside of the bracket. It seems to get confused about which side of the bracket the entry should be, and doesnt see that there was a mirror operation.

Do I have to rebuild this part right handed from scratch?

Thanks,
Colin

[guru_florida]

Well, I have something new. By right clicking on the series in the Group box, I got a Flip option. It flips the bolts around and they now go through the holes properly, and mate properly, but they are entering the wrong side of the hole. I really need to flip them the other way, but if I do, they go back to being oddly not going through the holes at all just resting up against them on the bolt head.

C

[mcArch]

What machine are you talking about?, What program?
-- Mike

[Aley]

I've never had much luck with smart fasteners. In your assembly, why don't you use the mirrored bracket and manually add the fasteners from the toolbox, adding appropriate mates as required? That'll give you the mirrored bracket with all its dependencies (which is extremely useful if you redesign the bracket), and still keep your assembly, exploded views, and BOM accurate.

For me, I never use smart fasteners anyway - I just add things from Toolbox, and depending on the fasteners I either let it automatically create the mates as I drag in the fasteners, or I drag them unmated into the assembly and use the Mate tool to add the mates I want. (I usually do the latter on flathead screws, where I prefer to use a Coincident mate between the conical surface of the countersink and the conical surface of the screw, which is not the default.)

[DareBee]

I have to agree with Aley.
I would think it would be much more important for your mirrored part to be linked to the original so that changes will propogate.
Fasteners have no purpose in assemblies other than to add mass and look pretty.

[guru_florida]

Thanks for the direction, Aley and DareBee. I agree, the bracket linking is more important to me. I thought maybe I was missing something with the smart fasteners. I will use the toolbox and place them myself.

DareBee: I can think of one advantage to placing the bolts! Up until now I was mating without bolts for the same reason you state. Then when I built the machine I realized two of my parts interfered because of the bolt heads. I didnt see it in the model because it was within the machine but collision detection and probably myself would have noticed if I had placed the bolts. Kind of changed my opinion at that point!

One other question if I may: Do you create many parts within the assembly itself, thus having relations to existing parts in the assembly. At first, I used this, but at some point I stopped because it seemed to cause a lot of trouble. On the flip side, having relations accross parts certainly helps make, for example, mounting plates where the mounting holes can be changed easily and changes cascade via relations. So I am beginning to rethink revisiting cross part relations and perhaps my initial trouble was more user error and my incompetance using parametric design. Now I do mind my mates carefully and keep my sketches properly defined. I have very little rebuild errors ever, and I let none persist.

C

[DareBee]

Top down design is what I use most. That way when you change 1 part they all fix themselves. This is the reason that I do most of my holes using the "Hole Series" feature as well.
I do model purchased components or existing tooling separately.
I rarely use Smart fasteners. Where applicable I use on-size holes for locating fits, smart fastener will not put an 8mm screw in an 8mm hole. Occasionally I have to mix imperial and metric fasteners in the same part and it really doesn't like that either. I also dislike that I have to open the smart fasteners and "mark them up to date" every time I change something on the model.
Inserting from toolbox is a single click per screw so I usually go that way.

[guru_florida]

I have gone through a lot of my assemblies and I have made a lot of headway in the last few hours. I was already going top down hierarchy with assembies, sub-assemblies, and parts. This is a model of a moving table cnc-machine, the two table axis are a single sub-assembly, then the Z-axis assembly. Even the ballscrew+nut, and rail+bearing-blocks, etc, are thier own assembly with proper mates.

In the last few hours I have used the toolbox to insert the bolts. With a little practise it is super-easy! All my bolts are inserted now.

I have also redone some of the hole wizard sketches, so they now reference other parts. My mating holes are now more parameterized. I also, redid the Z-axis mating, removing a lot of dimensions and referencing other parts in the assembly. Now if I adjust the distance of two bolt holes that hold the Z axis linear rail the linear rails will move apart (or closer) and all parts like the bearing blocks, carriage, etc, will update. Nice!

Some other tweaks too, cross part references are working good for me now!

btw: Another useful thing about placing your bolts is having them listed in your BOM with correct sizes.

Thanks,
C

[cam1]

Not to be an annoyance, but the use of the top down terms used is not entirely correct. You are really referring to the organizational hierarchy of your assembly, not the methodology by which it was designed.
Top down design is a method of design that designs parts around existing parts. An example of this is a house who's roof is designed first, after which the walls etc are designed.The roof drives the shape of ther house.This method is typical in some shops where the customer supplies the part, and you design the fixture.

Bottom up design is the more "traditional" method, which as it implies, designs an assembly starting from the bottom up. Using the house as an example, the foundation is first designed, the shape of the roof is dictated by the shape of the walls.

As far as smart fasteners go, I usually just add 1 bolt/feature, to make sure that I've selected the correct fastener and stack up. After that, I just enetr the number manually into the BOM. I find that fasteners in large numbers are visually pleasing, but really take up alot of memory.

regards

[DareBee]

To make sure we are all clear
Top down and bottom up have NOTHING to do with the direction of build.
Like Cam mentions, I design a lot of machines that run a specific part. I model the part and IN the assembly environment my tooling (etc) is designed directly from the features of the part.
Change the part and the machine/tooling automatically adjusts part geometry or location. Having parts adjust using mates is more typical of bottom up design.

[guru_florida]

I read an article on bottoms-up versus top-down that clarified my understanding of it. I was clearly using bottom up strategy before now.
After my changes yesterday I would say I now use a little of both, which I think is appropriate for each of thier case. Though I still have some changes to make, its looking much better.

With all the bolts in place, the model sure is a lot slower. I placed the bolts in sub-folders so I can easily supress but I am not sure how much this is helping speed things up. I think I will create a configuration "Fully bolted" and suppress bolts in the default config. This should give me my speed back right? I have 4GB of memory. (tho only 3.3GB recognized by 32bit xp, and I think only 2GB allowed per process.) I also think I can set a few sub-assemblies to lightweight.

cam1: I appreciate your input.

btw: A little trivia for you. Did you know that the recent "21" movie, based on a true story, was based around the guy that created the Solidworks Corp. Back in circa 93 he used the near million dollars he won playing Blackjack to create the Solidworks corporation.

C

[guru_florida]

At the risk of asking too many questions, and now being off the initial topic...

I have my rails and bearing blocks as an assembly. Then two of these are places as sub-assemblies to the axis assembly. Then this is a sub-assembly of the overall machine. I have set the sub-assemblies to flexible so I can test the movement of the machine.

However, based on some recent reading, perhaps I should have the carriage with bearing blocks as an assembly, then the ball screw/bearings as an assembly, and the static axis assembly. Then in the top level mate them together. This way the subassemblies stay rigid/fixed. Would this improve my performance, especially the responsiveness to grabbing the carriage with the mouse and testing movement?

Basically, does seperating my assemblies bound to parts that dont move in relation to each other improve performance?

(I included a rendered pic just for fun.)