Help understanding constraints.

Well,... im reading through my book and trying out what I read. Now I am feeling a bit overwhelmed with the geometric constraints. I mean,... I know that INV will tell you if your overconstrain something. But my question is,... how far do you go to contrain something?

I mean, should I contrain EVERYTHING that is horizontal, EVERYTHING that is vertical, that is equal, perpendicular, parallel, etc? That seems a bit much.

Do I constrain everything?!?! Is that what fully constrained means? Once again my book doesnt explain why, just how.

Do I have to fully constrain?!?! What would happen if I had a shape that was final with no constraints? I mean as long as I didnt try and reshape it,... it shouldn't move right? I dont see why it would.

I dont know. Thanks in advance.

... I dont see why it would.

I think every designer should work out on the shop floor for 4 years before being allowed to use a CAD software.

Of course you need to constrain everything.

A machinist doesn't just plop a piece of stock into a vise on the mill and start cutting.

If you have Inventor set up corrrectly then your horizontal, vertical, perpendicular, coincident, parallel and most tangent constraints should be applied by Inventor automatically. No extra work on your part. None. Simple. Robust and professional.

All you need to do is add the dimensions.

You should read this document http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf

If you don't want to fully define the sketch then don't, you can still extrude and loft ect and make 3d models, if you are using this in manufacturing and want to model a prototype or model a part to be built then generate 2d drawings for the shopfloor, or send the model to a cnc machine then I would build the model correct and constrain everything.

Thanks guys. Well,... what I meant really was, for example say you have a square. I thought I had to apply horizontal constraints for the top and bottom line along with parallel and equal constraints too. Some for the left and right except I would use vertical constraints instead. Oh and perpendicular contraints too. Thats a lot of constraining.

After playing around with inv some move I noticed that you dont have to apply EVERY constraint to fully constrain something.

Using the box and other tools similar automatically applies constraints too. I started off with the line tool. It applies contraints but not all of them. Atleast to my knowledge as of now.

I also noticed that the equal constraint ignores angles. I think it's meant for length only. Thats fine.

I'm getting the hang of it. Im reading through your "be a an inv professor in 90 minutes" before I continue through my book.

The one thing I like about inv so far is that it forces you to create dimensions. I was very bad at that with SU and AC.

Anyways. Thanks Professor:)

Ahhh and another thing,... I created a 6 sided polygon using the polygon tool and it said I needed 2 dimensions. So I gave one of the sides a dimension which left me with one last dimension that needed to be placed. But for the life of me I couldnt figure out what needed a dimension?!?!?

But for the life of me I couldnt figure out what needed a dimension?!?!?

Think of dimensions and constraints as the same thing. The dimension type of constraint designates magnitude, the geometric constraints remove degrees of freedom.

With your polygon click and drag one of the corner vertex points. You will find that it rotates around the origin (you did constrain the center point to the origin?).

This should give obvious indication of what is needed. Add a horizontal or vertical constraint to one of the sides.

If you are using Inventor 2009 or later you might want to right click in the graphics window while in sketch mode and select Show All Degrees of Freedom. You will get a red arrow(s) at any vertex with a remaining degree of freedom that needs to be constained for full control when editing (and I've never done anything of any significance exactly correct the first time - thus editing will be needed and thus constraining will make the editing predictable).

Thanks. Will give that a try.

I was about to say that I would be abel to fully constrain something using only dimensions but the polygon example shows that I cant. I can draw a box or something similar and specify a length for each side. by doing that I wouldnt need perp, vert, horz, para, equal, etc constraints. But as said the box would still be able to rotate or something else for sure.

But im thinking that by using the geometric constraints it would cut done on how many visible dimensions there would be therefore cutting down on screen clutter.

I think I will try and copy the model I did in AC09 using inventor now. Beytter yet I think I do that muffin pan exercise in your pdf you linked me before.

There were two thinkgs I didnt understand in that pdf. I forgot which ones. I will find out and post them later. Maybe you can explain. The explainations are very simple and quick. Which is good. I love it. Cuts out all of the BS and gets right to the stuff I need to know.

Thank you sir.

When I went on my first Inventor course, constraining objects early in the model was very much a feature of the instruction. The first constraints that we would apply (and I still do) were the horizontal and vertical constraints to the origin (center point in the sketch window) I find that doing that makes further work on the model more predictable. Many constraints (parallel, perpendicular for example) are applied automatically.

If you constrain in the vertical and horizontal, as soon as you do the dimensions you'll notice that the lines change colour to indicate a fully constrained figure.

I find construction lines useful for stuff like symmetrical shapes, using them as a mirror line. Center lines of course are the line of choice when defining the centerline of a sketch that I am going to revolve.

Keep at it, and don't tear too much hair out!

Yea im really starting to get the hang of it now. So far I can safely say that I like it more than AC09 atleast for 3D modeling. I havent used both enough to really pick out the good and bads.

But so far some of the goods are that you have to dimension. In AC you dont have to and neither in SU. I was bad with that. Constantly measuring stuff over and over. Another is that it saves your sketch seperate from the model your building. Another is threading. Quick! Easy! It's a material! I think it is. It's not real threading but it's good enough and saves on file size!

But that brings a question forward though. Say I model a bolt and a hole both with the same threading. Should the diameter of the bolt and hole be the same?!?! Or should the diameters for each be what they are before actual threading? You know what I mean? the bolt should be a diameter that reflects the major of the thread and the hole with a diamter that reflects the minor for the thread? If I do that the model of the bolt wont fit into the hole.

Wow this is eating at me now,...

Threading, as you say, is a breeze in Inventor. If you are threading a shaft just make it the nominal diameter; say 1/2 inch in imperial or 16mm in the devil's measure as a for instance. The dialog box allows you to select thread systems, even to changing nominal diameters!

Threaded holes are great too. No need to read through Machinery's Handbook for correct drill sizes, just use the threaded holes section of the hole generator tool, same thing for clearance holes for the bolt to pass through.

In the idw file, you may have to check the box to show thread details before the correct thread convention shows in the 2D drawing, and I always have to manually add thread notes, but that's a small thing and even that may turn out to be pilot error on my part!

Thats one thing I noticed. INV didnt have leave thread specs in the model. It;s so good at leaving dimensions for everything else you would think it would have something for threads.

Not to familiar with IDW files just yet. Still working on ipt files. lol.

Hey, how do you organize all your files for a model?!?!? Do you dump all the files for a model right into one folder or do you create a seperate folders for type of part?

I'm trying to create a standard for myself. I usually create a main model folder and then subfolders for the different parts. Just in case I create variations of each part,... color features etc. You know what I mean? So if im model a 20oz bottle of coke. I'll have a sub folder called bottle and another that says cap.

Whats a good habit, all in one folder and subfolders?!?!

Oh and I do carry a machinist handbook with me:\ im such a geek.

I'm a single user, and installed Inv 2008 as a single user, but I use the vault with a single project to make file resolution more sure. It's a bit of a fiddle-faddle to set up, but once done it's a very good way of organising all those files that you'll be creating.

There is a blog on this subject giving step-by-step instructions on how to do it. Go to the manufacturing community part of autodesk.com. Find the blogs of Brian Schanen. The instructions are in two parts, part 1 was written in May 2008 and part 2 was written, errr, a bit later (I can't find the date on the printout!)

The way it works is that you will end up using the vault like a member of a design team, not a problem at all once you get used to it. All your work will be in a single project with a folder for each of your designs, rather like using My Documents in Windows.

I used to make a new project for each design, but I started to get file resolution problems and I tripped up over this better method whilst browsing the Autodesk website for answers.

It sounds as though this method will dovetail quite well with your existing way of working with folders and sub-folders. Working this way also helps if you want to pinch a part that you made earlier to place in a later entirely seperate design without any file resolution hiccups.

The only thing you need to remember is to add files to the vault after you create them, the blog does mention it but I initially overlooked that necessity.

Do not add threads to holes like you do to shafts. Have Inventor automatically look up the tap drill size by using the Thread type hole in the Hole feature dialog box.

Because it places the hole smaller there will be interference between assembled fastener and hole (fastener isn't going to just drop into the hole with no thread engagement).

When it comes time to do the drawing you don't manually enter the thread note - use the Hole/Thread Notes dimension tool and Inventor automatically picks up the thread information from the model.

see attached

So I cant thread holes!?!? INv makes the hole smaller than the shaft of the same nominal size? Thats sucks. So I guess I could have two file of a part like that I guess. One with tapped holes showing the part not in use and one without threads for using the part in an assembly.

So about vault,... I will doubt that I will want to go through all that. I think. So you are saying that if I do the subfolder way and even share files with other projects I will run into a lot of problems? Im in a situation now where I need to create a part(o-ring) that will be used within several projects. Thats going to be a problem?

Thanks for your help guys.

So I cant thread holes!?!? INv makes the hole smaller than the shaft of the same nominal size? Thats sucks.

Of course you can.

Have you ever taken a basic machine shop class? The hole has to be smaller than the shaft or there will not be any material to cut the thread with a tap. This is called the tap drill size. You've got a long long long way to go.

Of course you can.

 

Have you ever taken a basic machine shop class? The hole has to be smaller than the shaft or there will not be any material to cut the thread with a tap. This is called the tap drill size. You've got a long long long way to go.

Oh yea I know that. The bolt diamter is roughly the major of the thread and the hole diameter is roughly the minor ofthe thread.

But in INV,... if I thread a hole at a certain size using the hole feature and then go ahead a thread a bolt for that certain thread size using the thread feature,.... the diameters for each will be different? Thats what your saying right?

If thats true,... I can say I like it becuse it's accurate but at the same time I dont because as you said before, there will be interference between the two if I put the bolt in the hole. That would leave me with having to keep the hole unthreaded with the bolts diameter.

Hmmm. SAy I did it anyways and animated the boly screwing into or atleast sliding in and out of the hole. Would it do it without problems if there was interference?

Oh yea I know that. The bolt diamter is roughly the major of the thread and the hole diameter is roughly the minor ofthe thread.

 

But in INV,... if I thread a hole at a certain size using the hole feature and then go ahead a thread a bolt for that certain thread size using the thread feature,.... the diameters for each will be different? Thats what your saying right?

 

If thats true,... I can say I like it becuse it's accurate but at the same time I dont because as you said before, there will be interference between the two if I put the bolt in the hole. That would leave me with having to keep the hole unthreaded with the bolts diameter.

 

Hmmm. SAy I did it anyways and animated the boly screwing into or atleast sliding in and out of the hole. Would it do it without problems if there was interference?

Doing a threaded hole is actually a lot more straightforward than that in INV. In your workshop, in the metal, you're going to have to drill the right size hole in accordance with the recommended tapping drill size. In Inventor, using the hole tool, you just place your hole center as required, select the threaded hole option, specify the thread in the dialog box, set the depth, and that's it, the program does it, including simulating the thread in the model. It's rather nice. JDM's screenshot is of the hole tool dialog box showing the threaded hole option selected.

On assembly, the insert option just fits the bolt into the hole no worries, as long as you're not fitting a 3/4" bolt into a 1/2" hole of course!

In the 2D drawing file, as JDM also advises, the thread details for the hole are picked up by the hole/thread notes tool from the model. It's left to the technician on the shop floor to refer to his tables to pick the correct drill, us designers just say what thread size we intend.

Hope this helps

AWESOME! Thats what I wanted to to know. Thanks:)

Dont mean to pick your brain but I have another question. About the o-ring I said I was going to have to make and share with several models,... when it's comes to accuracy, how would one go about making a o-ring thats fitted?

Making an completely unused o-ring is fairly easy. But what about a fitted o-ring? Fitted meaning I slid it onto a shaft. What im trying to say is that when you fit an o-ring onto something you are most likely stretching it out a bit which decreases the diameter of the o-ring a bit. Plus the area of the o-ring that comes into contact with whatever is compressed or mashed a bit decreasing the height in which the o-ring protrudes off the whatever. You know what I mean? And even worse,... a fully used or compressed o-ring in use! For given space,... how do I know what the shape will be at a compressed state?

I am thinking that I and going to deep into it but at the same time I dont think so. I need to know how much clearence is need for a given o-ring size. So this is kind of important.

Thanks again:)

So how I does a pro model an o-ring for fitment?

AWESOME! Thats what I wanted to to know. Thanks:)

 

Dont mean to pick your brain but I have another question. About the o-ring I said I was going to have to make and share with several models,... when it's comes to accuracy, how would one go about making a o-ring thats fitted?

 

Making an completely unused o-ring is fairly easy. But what about a fitted o-ring? Fitted meaning I slid it onto a shaft. What im trying to say is that when you fit an o-ring onto something you are most likely stretching it out a bit which decreases the diameter of the o-ring a bit. Plus the area of the o-ring that comes into contact with whatever is compressed or mashed a bit decreasing the height in which the o-ring protrudes off the whatever. You know what I mean? And even worse,... a fully used or compressed o-ring in use! For given space,... how do I know what the shape will be at a compressed state?

 

I am thinking that I and going to deep into it but at the same time I dont think so. I need to know how much clearence is need for a given o-ring size. So this is kind of important.

 

Thanks again:)

 

So how I does a pro model an o-ring for fitment?

I sweated a bit on this one and gave up on it for a while to do some work!

To experiment, I modelled a shaft 22mm dia with a 1.8 x 1.8mm square groove around it as a gland for the "O" ring. Then I pulled an ISO O ring from the Shaft Parts > Sealing > O-Rings section of the Content Center, using the Table View tab to size the O ring. Thus far, no problem. It was the assembly that I had an attack of the dumbs over.

I've just had another go, and they've gone together OK now. I used a mate constraint between an axial face of the gland/groove and the O ring. This make the two parts make contact, but at any old angle. I then went into the Model Browser, expanded the Origin of the O ring, made the YZ plane of the O ring visible, and made a 0.0 degrees angle constraint between the plane and the axial face of the gland. Voila, c'est parfait as they say across the ditch (from me, across the big pond from you).

Hope this helps, and my apologies for the delay.

John

I sweated a bit on this one and gave up on it for a while to do some work!

 

To experiment, I modelled a shaft 22mm dia with a 1.8 x 1.8mm square groove around it as a gland for the "O" ring. Then I pulled an ISO O ring from the Shaft Parts > Sealing > O-Rings section of the Content Center, using the Table View tab to size the O ring. Thus far, no problem. It was the assembly that I had an attack of the dumbs over.

 

I've just had another go, and they've gone together OK now. I used a mate constraint between an axial face of the gland/groove and the O ring. This make the two parts make contact, but at any old angle. I then went into the Model Browser, expanded the Origin of the O ring, made the YZ plane of the O ring visible, and made a 0.0 degrees angle constraint between the plane and the axial face of the gland. Voila, c'est parfait as they say across the ditch (from me, across the big pond from you).

 

Hope this helps, and my apologies for the delay.

 

John

Awesome! I have to try this out. I'll let you know:)