gears

Can someone help me. I took a blue print of a gearbox from the white pages and making it in inventor and i came to the part of gears and i was wondering if anyone can help me with these gear or knows of a place were i can download the gears.

Dual-Motor, Dual-Speed Robot Transmission

the gears are:
Speed change gear 20 pitch, 20° pressure angle, 1/2” face width, 25 tooth steel gear B-GSS-2025 Small Parts

Bosch pitch change gear 0.7 module, 20° pressure angle, 1/2” face width, 55 tooth steel gear MSG25-55 PIC Designs

Torque gear A 20 pitch, 20° pressure angle, 1/2” face width, 14 tooth steel gear B-GSS-2014 Small Parts

Torque gear B 20 pitch, 20° pressure angle, 1/2” face width, 50 tooth steel gear B-GSS-2050 Small Parts

Torque gear C 20 pitch, 20° pressure angle, 1/2” face width, 25 tooth steel gear B-GSS-2025 Small Parts

Torque gear D 20 pitch, 20° pressure angle, 1/2” face width, 40 tooth steel gear B-GSS-2040 Small Parts

High speed output gear 20 pitch, 20° pressure angle, 1/2” face width, 35 tooth steel gear B-GSS-2035 Small Parts

Shifting gear high speed 20 pitch, 20° pressure angle, 40 tooth steel (303) gear stock A 1C29-Y20040 Stock Drive Products

Low speed output gear 20 pitch, 20° pressure angle, 1/2” face width, 15 tooth steel gear B-GSS-2015 Small Parts

Shifting gear low speed 20 pitch, 20° pressure angle, 1/2” face width, 60 tooth steel gear B-GSS-2060 Small Parts

Try www.bostongear.com
They have 3d models of all their products in the BostonSpec section of their website. You can probably find gears similar to the ones you’re looking at.

JV

thanks i will check it out and see what i can find.

I don’t understand, why do people model gears more accurately than a cylinder? Is it just for looks, or is there some functional reason for adding alll those polygons? I must be missing out on something…

Try this as well.

I do it for looks.

When I’m messing around I throw in 2 different gear “cylinders”. One which shows pitch diameter (to model spacing), and one which shows OD (to check for interferences).

After I finish a design, I drop in the B.G. “accurate” models for looks. Why not? They’re already drawn up.

This goes along with “it’s not what you say, but how you say it.”
Sometimes a little flash along with your substance can go a long way. (As long as you still have a lot of substance ;).)

I always use “real” gears in my models just because it looks nicer. Also, if you’re planning on submitting an Inventor award, a transmission with real gears is going to look 1,000 times better than one with just cylinders.

There actually was one time I didn’t use real gears, and that was because I was on an incredibly slow computer and it didnt like all the details very much.

Cory

(reading back through this, you gotta be a CAD user to really understand what I am talking about here… hopefully, it is clear)

Here is how I handle gears in Unigraphics. Other CAD packages might have these features, I don’t know.

I made a parametric gear model about 3-4 years ago, and I just keep using it when needed. It took a few hours to set up, but I have used it countless times since that point.

The file contains 2 solid models, right on top of each other.

One solid is generated from an intricate sketch that outlines the actual gear teeth. This sketch is parametric, so I can change its parameters (# of teeth, thickness, pitch, etc.). When I change these variables, I get a gear with the proper pitch diameter, correct # of teeth, etc. I can also change the bore size with a variable.

The other solid is a simple cylinder that is created from dimensions calculated from the variables in the above solid. It automatically gets the same thickness, pitch diameter, and bore size that the “actual” gear has.

Since these models are solid, I can whittle on them if I need to put in a hex hole or a pocket, depending on my application.

Then, when I am working in my assembly, I import this gear into the assembled model. UG has a “reference set” feature where I can assign one model in a part to a named reference set. In this case, I have “actual” and “block” reference sets. While working in the assembly, if I turn on “actual” for that gear, I see teeth. If I turn on “block”, then it shows a cylinder. In the assembly, I use block reference set most of the time, until I want to make fancy pictures.

This is also nice for dimensioning. All of my detail prints are 1-part assemblies of the part getting dimensions (UG calls it master-modeling). So, when detailing the part, I pull in the “actual” reference set and the print shows the gear teeth. There are other reasons for master-modeling, but this is one advantage.

I am spoiled on Unigraphics. I assume that other CAD systems can do these things. Is this true?

Andy B.

I’m not sure if CATIA has an equivalent to the reference set. It has other features that might make it irrelevant. For example if I wanted gear teeth to disappear, I could just turn the feature that created them “off”. They would still be there but wouldn’t show up on any pictures or view until you turned it back on. Maybe the next time I visit you can show me what you mean.

Unless I’m actually creating a gear from the model, I usually don’t bother with accurate teeth. Notice I did NOT say I don’t bother with teeth. I simulate teeth using a trapezoid sized so the addendum and dedendum are right in relation to the pitch circle. This way I can check for interferences and clearances without a lot of extra data in the model. But it still looks like the gears are “real”. Involute splines for the teeth generally aren’t needed and in many systems cause the model size to inflate drastically.

I have made gears using a Selective Laser Sintering machine. This creates parts directly from powder using a file generated from a CAD model. These days just about any CAD system will create the required .stl file. For these I did have to model the involutes and they came out great. But I only did so because it was essential to getting the part to come out right.

ChrisH

not sure how much this will help you… but you might get some help here… :slight_smile:

http://www.firstcadlibrary.com/

This is also a great resource for Inventor users

On the website listed by Cory and Joshua May is an iPart for the gears you list. It is what I used when modeling the 2003 and 2004 gearboxes for our team.

I’m not sure if anybody has told you this already but I know a simple way to create gears (I made all of the 103 gears this year and I think they cam out pretty well). What you do is count the number of teeth on the gear (Number A). Measure the diameter of the gear (number d). Then you divide 360 over how many teeth you have. Make an arc with that degree. Then place a line down the center of the arc (so that the line goes far beyond the arc). Then you make a tooth from the center of the line but leaveing space on eath of the arc. You delete the extra lines and use a circular pattern inserting the number of teeth as your number of times repeating. It’s a bit complicated but after you do it the first time it gets pretty easy (I’ve made about 6 or 7 different ones) :confused: