Transitioning to Inventor from a Lightwave / Modo background

[Bishop]

Okay, I've been using Lightwave 3D for almost 10 years now, and I've got a fair amount of practical expertise with it, and I've been using Modo (it's wonderful b$%^@%d stepchild) for several months as well. Now, I've got a pretty hefty financial incentive to add Inventor to my arsenal, but I've got to get up to speed pretty quickly if I'm going to be able to take advantage of it.

 

A friend of mine needs to spend more time running his company instead of doing the pre-vis work, and so he's provided me with a copy of Inventor Pro 2009. I have virtually zero background with Autodesk products. I tried messing around with 3DS Max a year or so back, and couldn't wrap my brain around it, but then, there was no particular incentive to do so. I tried one of the LT versions of Autocad back in college in '95 or '96, but never really did anything with it - I was a poli-sci major, just messing around, so no classes.

 

I've had a look at some of the tutorials on JD Mather's site - thanks much for posting those, btw - but I'm still having trouble with just the basic concepts of 2d / 3d sketches, and making a part. It's just such a different workflow from the 3D packages that I'm used to using.

 

Any suggestions on specific tutorials and info for transitioning from my sort of background, vice an AutoCAD (or other CAD package) background? Most of what I've found out there has been for people who already have used AutoCAD extensively ...

 

 

 

Thanks!

[shift1313]

welcome aboard. The modeling approach for something like Acad will be different from a software package like inventor. Do you have a specific example of something you would draw? that might help lay out the ground work and planning that goes into the model.

 

A basic understanding of the tools available to you will probably be a good start. the help files are full of info as well as tutorials for you. Basic operations like Extrude, Revolve, Sweep and Loft are the basis for most of the modeling. For 2d, you are restricted to a plane, either one you create or one of the 3 origin planes. From here you can use your open or closed sketch to create your features. 3d sketching opens up a new can of worms. You have to understand your tools and what they can do to be able to use your sketching environments wisely.

 

For instance you can create a lofted surface using 4 3d sketches(intersecting). From there you can thicken that surface to make it a solid, but you cannot extrude a non-planar sketch.

 

If you give us an idea of what you will be drawing we can point you in the right direction

[Bishop]

Well, to start off with, the stuff that I'll be working on later has nothing really to do with what I'm doing now - I'm just trying to figure out how this all sort of works. I'll be mostly doing piping / valving systems, maybe some custom design of mounting hardware and flanges, and deconflicting installations with what the customer already has.

 

For the moment though, I've just been kind of playing around with an idea for a .22 bolt action rifle receiver. Nothing complicated, just a simple tube, about 1" diameter, 4" long, with some cuts in it for parts, and threads at one end for the barrel.

 

I've discovered the trim feature, and how I can lay out several different shapes in a 2D sketch and just cut away the bits that I don't need, and that's pretty nifty. I'm having some trouble with the 3D sketch stuff, though. In 2D, I've got everything snapping to my grid just fine, but it doesn't seem to do that in 3D. Also, is there any way to, rather than suppress the features while I lay out another sketch, just make it show up as a wireframe, so I can see what's going on for orientation purposes?

 

The help files and such are supremely non-helpful, so far ...

[shift1313]

Well the reason I asked what you were going to work on was because Inventor has many built in features to speed things up. For instance there is a tube/pipe routing application built in. Content Center has loads of common pipes, fittings etc. Also there are loads of common shapes that you can insert into your drawing for cut outs, or other features.

 

One thing i should mention is when creating your files you are presented with several options. .ipt is a part file. a single body(inventor 2010 allows multibody parts but i dont think 09 did, jd mathers would know). .iam is an assembly file. Inside the assembly file you can Place .ipt files or create them as you go. When working with assemblies, when you edit one part, all the rest go dim/transparent so you can see what you are doing. Also you can right click on them, or on their name in the model tree and change their visibility if needed.

 

From the View tab you can change the solid models from Shaded to Hidden lines or Wireframe view.

 

When working in the sketch environment(2d or 3d) the bottom right of your window will tell you if more dimensions are needed to define the sketch. Sketch lines are green when under-defined and turn black when fully defined. Its important that you understand this. Did you go through JDs tutorials? Sketch dimensions, projected geometry and constraints are the basis for modeling. Skipping these will cause you some big headaches down the road. Especially when you need to change something in an assembly file.

 

I turn grid snap off when i model so i dont know about snapping in 3d. When i start a sketch(2d or 3d) i make sure to use the origin or another reference point to start. Lay one line, or circle down and add a dimension before I continue. I make use of creating reference lines and centerlines(especially for revolved features). If you roughly sketch things how you want them, there is an Auto Dimension feature. It will automatically create dimensions for the sketches current position/location. you can edit these dimensions.

 

 

Ive added a few images that may help(hopefully). The first one shows the difference between a fully defined line and one thats under-defined. The black line has a vertical constraint, a coincident constraint with the origin and a dimension of 4". the line off to the right has nothing so i could drag/pull it around the screen.

 

second image shows you the centerline tool(and just above it is reference line). You can select a line(my 4" vertical line in this case) and make it a centerline. dashed centerlines and reference lines wont be considered when performing operations like extrude, sweep etc.

 

3rd image shows the view tab with shaded,hidden and wireframe options.

 

4th image shows a fully defined sketch that im going to use for a revolve feature. note the 2" dimension at the bottom appears to reference nothing. When using the centerline option, your dimensions added are are full width. this isnt only helpful for revolve features but other things as well. especially when creating symetrical parts where you want to draw half, then mirror about this centerline.

 

last is a section view of my revolved feature. you will also notice on the Model tab there is a Thread option that adds cosmetic threads. if you wish to actually cut threads you will need to create a helix and sweep-cut a thread profile from your part.

[Bishop]

I have been working through some of the stuff from JD Mathers' site, but unfortunately there seems to be an expectation of a higher starting-out point, knowledge-wise, than what I've got.

 

Okay, here's a specific problem I'm having.

 

I basically gave up (for the moment) on creating complex shapes and just made two very simple flanges with a gasket in between them. (I've attached the IPT and IAM files here.)

 

I've got them mated together, and it looks like everything is lined up correctly. However ... when I attempt to make a bolted connection between them ... that's when the fun starts.

 

1. If I use linear, it works. It cuts a whole extra hole, which would pretty well destroy the utility of the flanges ... but it works.

 

2. If I use concentric, it doesn't work. I select the top and bottom planes (top of flange, bottom of flange2), and I can select one circular reference ... but I think I'm supposed to select -all- the circles that the bolt passes through. I can't, though. I can only select one reference. Whether it's the hole in flange one, the hole in the gasket, or the hole in flange2, I can only select one, and I don't get any fasteners to choose from in the right side window.

 

3. If I use the hole option, I can only select the top and bottom planes. It won't actually recognize the holes as, well, holes.

 

 

What'm I doing wrong here?

part1.zip

part2.zip

[JD Mather]

flange.ipt

Your first sketch is not constrained - read these documents (slightly different - read both and get the example files).

http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf

http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

 

Do not use circles for your threaded holes. You used the wrong size circles for the holes - there will not be any material for your threads, the fasteners will fall into the holes. Using the hole feature tool will automatically select the tap drill size.

 

Do not use Move Face to change an extrusion distance - simply double click on the extrusion to change the distance. I have used Move Face maybe twice in the last 5 years, maybe.

[JD Mather]

flange2.ipt (see previous) You can have Inventor select correct clearance hole size for fasteners. You could do both chamfers as same feature.

[JD Mather]

assembly.iam

 

You could replace all of those assembly constraints with 2 Insert constraints (actually 4 - 2 for first two parts and then 2 for third part to first 2). I recommend selecting diagonal holes.

[Bishop]

Ah, okay. I didn't know about 'move face.' in the packages I'm used to, you just grab faces / edges / points and move them around as needed. The learning curve here looks like it will be pretty steep...

 

 

Thanks for the pointers!

[JD Mather]

... in the packages I'm used to, you just grab faces / edges / points and move them around as needed. The learning curve here looks like it will be pretty steep...

 

I could show you how to use Inventor in the same way, but that makes me shudder with nervousness. I have never used the other apps you refer to, but those sound like art apps. Inventor is an engineering app, and as a former machinist I shudder when artists start dragging stuff around without concern for manufacturability. I like nice clean dimensions matching the standard cutting tools I have.

 

Inventor is a professional tool and deserves a professional level of instructions and preparation - but a really bright person can probably do well by attaching files here and taking in constructive criticism. At times I can be a little tough - don't take it personally, I just take this stuff wayyyyy too seriously. So I've been told.

[Bishop]

I could show you how to use Inventor in the same way, but that makes me shudder with nervousness. I have never used the other apps you refer to, but those sound like art apps. Inventor is an engineering app, and as a former machinist I shudder when artists start dragging stuff around without concern for manufacturability. I like nice clean dimensions matching the standard cutting tools I have.

 

Inventor is a professional tool and deserves a professional level of instructions and preparation - but a really bright person can probably do well by attaching files here and taking in constructive criticism. At times I can be a little tough - don't take it personally, I just take this stuff wayyyyy too seriously. So I've been told.

 

Well, knowledge is what I'm after, and there's several hundred reasons a week for me to be good about criticism and teaching.

 

I want my work to be clean, not just for a client, but also for

myself, because one of the first things I plan to buy with his money is a CNC mill. Ease of manufacturing my parts will be important.

 

And yes, my other programs are primarily art programs. A lot of the CGI you see in movies and tv is done with those two. Good stuff, but not really engineering-oriented.

[shift1313]

one thing that you can do to help you understand dimensions and constraints in 2d is drag your sketches around. If you draw a circle on the screen then select its center point you can move it around. If you select the actual circle you will drag and increase/decrease its diameter. If you apply constraints such as vertical with the circle center point and the origin now the circle can only be moved up/down. If instead you apply an ordinate dimension from the origin to the circle you can now drag it around the origin with that dimension as your diameter and so on.

 

same thing with any sketch element. Depending on system settings, as you are sketching little icons will pop up next to your cursor with implied constraints. Things like parallel, perpendicular, vertical/horiz and so on. In the sketch environment the F8 key will display all constraints(F9 will hide them). when they are visible you can click on them and delete them if you like, for instance drawing lines and two snap to be perpendicular but thats not what you wanted. Simply delete that constraint and add an angular dimension between the two.

 

I wouldnt worry too much with .iam files until you have a firm foundation with fully defined sketches. I dont know of any large resources besides JDs tutorials and the stuff built in to the software and on the autodesk site. BUT specific questions can be answered and most of the time searching this forum will bring up results.

[kencaz]

I could show you how to use Inventor in the same way, but that makes me shudder with nervousness. I have never used the other apps you refer to, but those sound like art apps. Inventor is an engineering app, and as a former machinist I shudder when artists start dragging stuff around without concern for manufacturability. I like nice clean dimensions matching the standard cutting tools I have.

 

I beg to differ on this...

 

Inventor Fusion allows you to do just that. Push and pull faces and move holes without having to always go back to your history tree and edit your feature sketches.

 

 

I often times find that I can do a drawing of a mechanical part much faster in AutoCad then I could in Inventor, because I don't have to worry about constraining and history tree's. I just need to make the part.

 

Don't get me wrong I am an avid Inventor Fan and user and I use both that and AutoCad equally. I would not want to have to make a choice on which I would use if I had to get rid of one, but fortunately I don't have to make that choice yet.

 

I can't wait to use Inventor Fusion because of it's free form and parametric capabilities, but I curtinally would not call it an Art App...

 

 

 

KC

[JD Mather]

Inventor Fusion allows you to do just that. Push and pull faces and move holes without having to always go back to your history tree and edit your feature sketches.

 

Fusion scares the bejesus out of me. Not that I don't think that I can't use it - I know I will be fine. But in my experience 90% of CAD users (any program) don't have a clue what they are doing. At least with a history tree it can be discovered exactly where they went wrong and hopefully teach them something.

 

I often times find that I can do a drawing of a mechanical part much faster in AutoCad then I could in Inventor...

 

I consider myself one of the very best in AutoCAD. (ouch, put my shoulder out of joint) I can do most anything except schematics much much faster and better in Inventor than in AutoCAD.

[JD Mather]

I beg to differ on this...

 

I can't wait to use Inventor Fusion

 

Why are you waiting? It has been available for months, and for free!