@Anonymous wrote:
My extrusion cut will be maybe 3mm deep (the machined area). In inventor when I get to the "machining" tools, will they all be cutting tools kinda like what I just described here? In other words, in my weldment file should I be making all the plate parts out of normal stock size, or should I model in the cut, machined areas first and then the machined tools are just note type tools for the drawings?
Yes, they are modeling tools, organized into phases of the fabrication process as I described in my earlier post. The "Machining" environment consists of operations performed after weld. You can model your parts at the condition they would be in before assembly and weld, and then use the Machining environment to add post-weld cuts, holes, etc. There are drawing tools (in the Edit View dialog box) to show the assembly at the various phases, but the Machining environment itself is made up of modeling tools.
@Anonymous wrote:
With regards to multi-body modeling, what do you mean? How do I do this? From what I can tell at this point it looks like any tubing needs to be done in a weldment and assembly file. I can't just start an .ipt, draw a line, click on the design tab, and then click the line. In fact, if I remember right, the design tab isn't even in an .ipt file.
Multi-body modeling wouldn't necessarily apply to something involving tubing or other structural steel members. For that, you are better off using Frame Generator (on the Design tab). You are correct that this is an Assembly function. Multi-body modeling techniques can be used together with Frame Generator in the same assembly, but they aren't the same method.
@Anonymous wrote:
EDIT: I forgot to add; so how do I add holes in an assembly and keep them concentric with another part? In SW i mate the part where I want it and add my holes and constrain them to holes in the other part. These holes are then defined in part 1, let's say this is the weldment, based on the holes in part 2, let's say this is the cylinder. Now if I change mates between the cylinder and the weldment the holes follow. It almost looks like in inventor I have to measure the hole pattern on the cylinder, put it in my part, and then mate the cylinder threaded holes to the holes i cut in the weldment (stupid, stupid, stupid). I guess you could argue that the mates will make sure the holes stay related, but this isn't convenient.
You can do something very similar in Inventor. I skipped responding to this portion of your original question because I didn't want to overcomplicate my explanations at the time. Although it is possible to achieve what you want via a couple of different methods, my suggestion would be to initially do it the longer, more manual way of manually adding the holes in your weldment, until you have a better grasp on the basic functionality of Inventor. Then come back and learn additional techniques.
jordan.schroeder wrote:
This brings me to another point: updating. Today while working on a weldment I changed tubing size by making it smaller. The tubing had plates on both sides that were generated by mirroring the plates about the tube's mid plane. When I made the tube smaller the mirrored plate was floating in the air, the update lightening bolt wasn't green, and the refresh button in the manage tab didn't do anything. Why do I even have to worry about this? It should update on its own as soon as the tubing changes. There was a circle made of 2 arrows on the LH side of the original plate name in the design tree, but when I RMB'ed on it there wasn't any refresh option or anything.
This is something that actually is genuinely stupid. Forget you ever saw the Mirror command in the Assembly environment. It basically just mirrors the position of the component, and doesn't actually constrain it there. You need to constrain that second plate, probably using Symmetry constraints, rather than hoping the Mirror operation will keep it located properly (which it won't). Also, in some cases (rotational symmetry) you can use a Circular Pattern instead of Mirror, which would keep them associated as desired.
Some advice on a slightly different note: You said you spent the entire weekend trying to learn Inventor I have trained new engineers and even interns, some of whom were civil engineering students with no parametric modeling experience, and had them doing simple production work with welded steel fabrications in less than a day. For some of them, the only 3D experience they had involved an Xbox. Your problem with learning Inventor isn't with Inventor - it's with the way you are approaching learning it. Solidworks may handle some things better than Inventor. It could even be a hands-down better program. It could be free of all bugs and coded to perfection by the gods themselves on Mount Olympus. It wouldn't matter, because you don't have it anymore. Stop trying to force Inventor to conform to the way you're used to doing things in Solidworks, and then balking every time it requires you to do something differently than you're used to. Try to learn Inventor on its own terms first. You may still end up not liking it as much, but I think you'll have a much less frustrating time trying to learn it.
In other words, don't think of it as "This is how I did weldments in Solidworks, how do I do that same method in Inventor?". Think of it as "How do I use weldments in Inventor?". Leave Solidworks out of your thinking process as much as possible.
