For this reason amongst others I have been getting up to speed with Fusion 360 for the best part of 2 years now. Like any mid range CAD system, it has its annoyances - and as it's still in active development, there are still some key features that haven't been implemented yet. But right now it's pretty damned close to full featured - good enough for my needs at present. And it is free for hobby use, includes full 3D CAM and has a host of other stuff such as FEA, rendering, sheet metal, surfacing tools etc. Bargain buckets.
Whilst it is possible to import most CAD models into Fusion 360, there are some formats that haven't been catered for (eg Solid Edge, grrr). And even the formats that are supported lose content on the way in. So assemblies lose their mates / constraints / joints etc and the components lose the sketches that were used to define the basic geometry.
I know there are some errors in the existing SW models and I have also identified some changes / improvements that I'd like to make before I cut any metal. While it's possible to use "direct editing" to modify the imported models, without any underlying sketches, it's not easy to see what you've got to start with or to go back in and quickly change a dimension. And worse than that, there is no linking of components possible. With linked components, if you modify one, the changes flow through into the other. That's immensely helpful.
So, time to start over again. But with the existing models I imported into Fusion from SW, I can at least create 2D drawings in Fusion and use them identify the dimensions I'd come up with previously. Then I can create the basic sketches in Fusion to make "proper" models, complete with the various corrections and modifications I identified and the flexibility to make changes later without screwing everything up.
There are different ways to create models:
In Solid Edge "Synchronous Technology"(!!), you create a sketch, then when a 3D body is made from that sketch, the sketch completely disappears. In their terminology it is "consumed". That's because in ST, the model is a 3D body, not an extruded 2D form - the way I understand it.
In Solidworks (and Fusion and many others), you create a sketch, then make a 3D operation with it, either to create a new body or to modify an existing one. So you could make a body, sketch a feature, make a cut or extrude etc, make another sketch, perform another 3D operation etc and so on. Before long you have an endless stream of anonymous sketches and operations - and no clue where to edit that dimension you want to change.
Better method in my view is to aim to make a master sketch with as many dimensions and features defined as possible. Then you can easily modify those key dimensions without digging around endlessly to find the appropriate sketch.
Although the sketch is made hidden after a 3D operation is made from it, you can simply turn on visibility again, each time you want to reuse it to create further features.
Here goes - CAD model creation for the body, cover and mating bearing housing:
Master sketch for main bracket body. Almost all features are defined here:
First extrusion (walls):
Second extrusion (floor):
Cut extrude (counterbores and cover fixing holes):
Chamfers on rear face:
Final front view:
Final rear view:
Now make the cover by extruding from the bracket master sketch:
Final view with features added to cover (fixings, chamfers etc - 50% transparency):
Master sketch for bearing housing (part of existing machine - it mates with the bracket). Again, although the drawing is fairly busy, it defines the vast majority of the features in the final part.
Bearing housing final (after various extrusion / cut extrusion ops - 50% transparency). Obviously you need to supply the third dimensions at this point, to define the extrude operations:
Finally, putting these 3 parts together, we get the bracket, cover plate and bearing housing. There's more to the assembly than this but the other parts (pulleys, tensioner, ballscew, motor etc) are already defined. I will make Fusion parts for these at some point but apart from allowing me to make a complete assembly of the Y axis system, it doesn't move anything forward so can wait for now.
Now to go into the CAM environment. It's helpful to think through the machining operation carefully before diving into the machining operations.
This is actually quite a tricky part to machine, given the difficulty fixing the stock down and the near-complete coverage of the surface in terms of machining. You can't machine where the part is clamped. And as many operations as possible should be done at the same setup to avoid spending years aligning the features after each part move.
Originally I had the body dimensioned at 100mm width, to be machined from 4" x 1-1/2" stock. That would require 1.6mm total stock removal from the width - and provide a challenge on the workholding front. So I got pragmatic and changed the final dimension to 101.6mm. This would avoid me having to machine the sides. I measured the stock and it's pretty much bang on the 101.6mm size, so the chamfers etc should blend in nicely. If I want to finesse the surface finish, I can always use the belt sander etc.
My plan is to make the part from a longer piece of stock (to simplify clamping in the machine vise) and finally saw the extra length off right at the end. The final machining operation will then be to face off and chamfer the sawn end face, which should be simple enough to set up.
This approach would enable me to machine the tapered faces and the cavity in either sequence without needing to clamp down hard on a fragile part.
I think it makes sense to machine the taper profile, fixing holes, cylindrical bores and associated chamfers in one setup. Then turn it over and mill out the cavity. The remaining operations in this setup are fairly non-critical (hidden!).
My machining sequence is going to look like this:
- Face off the "bottom" of the stock (large face mill).
- Machine out the cylindrical bores (long series end mill), drill the bolt holes and mill out the tensioner slot (small end mill).
- Machine the tapered profile (long series end mill).
- Chamfer the edges and large bore (chamfer mill).
(turn the part right way up in the vise)
- Face off the top surface (large face mill).
- Machine out the cavity (long series end mill).
- Counterbore (mill) 2 large bolt holes (small end mill).
- Countersink the other 2 bolt holes (chamfer mill).
(remove and chop off extra length of stock)
- Face off / chamfer the sawn end face (long series end mill).
Firstly I need to model the stock. Without a sensible stock boundary defined, I could end up with the tool plunging into the stock just beyond the model. That could be exciting. You can use the stock model to define the machining boundary to avoid those buttock clenching moments.
Also, I should model some jaws. They can be defined as "fixtures" and Fusion will know to avoid them - or at least will flag up any tool clashes during simulation. I've got the toolholders modelled too, for the same reason.
First, create a model of the stock. This is positioned around the bracket model to give some excess stock around the edge of the model at the end and at the top and bottom. I've changed its transparency to 50% so I can see the bracket model within:
This is the stock - with added fixtures (jaws):
And finally, start setting up the CAM operations. This is the initial facing operation for the bottom face. You can see that the tool lead-in and lead-out are beyond the stock boundary, so it doesn't plan to plunge into the top of the stock(!):
To be continued....
No comments:
Post a Comment