Does anyone know if SW has an option to draw gears by filling in pressure angle...# of teeth...etc...
If you have SW Pro or Premium, you can use the Toolbox's library to drag&drop 3D approximations of gears into an assembly and use their geometry to create sketchs/parts/etc... The gears in the library aren't modeled as TRUE involutes, so you should not use this geometry for manufacturing, but if you just need the gears to look "good enough", then I have found them to be excellent.
Where I work we use a lot of gears and I use the toolbox parts as a baseline and then add whatever features I need to the part files. In our released drawings, we call out all the relevant gear data in the text.
I hope that makes sense.
To do this, in an new assembly, go to design library menu on the left and wade thru the folders to find the gear type you want. Drag it onto your assembly window and configure the size, etc...
Thanks! I was hoping for accurate details...
Karen, check out the Camnetics software. You can download a trial copy that lasts for about 2 - 3 weeks. Soildworks is pretty good for general visualization, but the tooth profiles are not accurate. When you mesh 2 gears there is a lot space between them so it gets quite confusing for a beginner to see if their gear train will work or not. On the other hand, gears generated by Camnetics mesh VERY close to the real thing so you can see much better what your assembly will look like. Once nice thing is that Camnetics generates a gear directly for Solidworks, no conversions are required. If you can afford it, I think the better option is to look at the GearTrax software, which is just a bit more sophisticated than the GearTeq.
If you need to create gears with accurate profiles etc, then take a look at the software called 'Gear Teq' or 'Gear Trax' Camnetics.
This is very accurate software and can generate all the commonly used gear types.... Software is about $1200 or so as I recall - very good.
Awesome...I'll give it a shot!
I don't know much about gears, but I use GearDXF. It makes 2D files of gears. Many options. Free to use.
awesome...i'll give it a shot
i just downloaded and tried this free software. It does generate a much more accurate tooth profile than Solidworks does, however since the tooth profiles are created using splines, it is fairly slow to extrude the gear to its final thickness. To make things faster, put in your sketches for the bore and the keyway. Apart from the slowness, the only drawback is that you only have the option of generating spur gears.
The Camnetics software does a variety of gears for you, although I guess you get what you pay for.
Thanks for the link Andrew.
It does generate a much more accurate tooth profile than Solidworks does
Curious statement. SolidWorks does what you tell it. Tell it to draw an involute and it will.
See my post in this thread.
Re: Parametric Spur Gear
It does generate a much more accurate tooth profile than Solidworks does
I don't know where you got that idea. If you check out the help listing for gears - it specifically says that the gears that are generated are NOT true involute gears and they are not to be used for manufacturing..... there is no option in the gear creation in the toolbox to 'tell' Solidworks to create an involute gear.
Maybe that ability exists in other places, but NOT for gears generated by the toolbox. It is certainly possible to create a spur gear using other methods but I dont understand why the average person would even consider that, spending a lot of time, for what the toolbox does in seconds. The toolbox version is good enough for most presentation work. If you need to be able to machine the gears or print them with a 3D printer, then dont use the toolbox profiles, the gears will be too loose.
I think that the Geardxf software would be accurate enough for 3D printing gears, however the Camnetics is more flexible and likely more accurate.
No... but my gears have involutes, generated in SolidWorks. SolidWorks is perfectly capable of generating involutes if one is inclined to do a little algebra and use an equation-driven curve.
So... your 3rd party application may fall short, but SolidWorks, properly implemented, does not.
Is there a parametric (equation driven) model of a standard spur gear out there?
One that has an involute tooth form driven by an equation with Global Variables?
I have down loaded and dissected various models, followed tutorial You Tube videos, built models and rebuilt models… But I found that some downloaded examples are not based on a true involute curve, some use several radii fit to points to approximate the curve, some adapt a spline curve to points. One I downloaded uses a formula in the equations to form an involute curve and the equation seems to work well when applied in the initial design/build of the model BUT breaks during the rebuild after changing say the tooth count to make a new gear. I have tried to reorder the equation solve sequence to no avail. I think it may have something to do with the use of a Global Variable in the definition in the parameters of the parametric “equation driven curve” for the involute form but am not sure.
All I would like is to have a model where I can change one or two Global Variables and have a new gear. Not too much to ask but the task seems daunting. I have even purchased a program that will give a export, in DXF, of a gear but its tooth form is an approximation of the curve using small straight line segments. I have trust that the form this program outputs is quite true and I use this program’s output to check and verify THAT the output from my various Solidworks modeling attempts matches it.
In the end I would like to have a model that has a set of equations that can figure/calculate the new gear with a true involute curve using the user input values for the pitch diameter, number of teeth and pressure angle. It should also be nice to have the ability for modifying, or deviating from the standard, for an extended addendum & dedendum.
OK. I said before I post the above lets Search the Solidworks forum using my post question as a Query.
And I found this very helpful thread. I would like to thank Roland Schwarz for his post to show me the way.
Now if I may, I did find Rolands' model to be a bit off, for when I modeled My gear using his technique,
The Involute Curve was off by .0007 I know that is not much but it was the idea of it. I had to find out why???
It seems using the definition in the parameters of the parametric “equation driven curve” in Solidworks
X(t) = "Dx@Sketchx"*0.5*(cos(t)+t*sin(t))
Y(t) = "Dx@Sketchx"*0.5*(sin(t)-t*cos(t))
This places the start of the curve on the y axis at the base circle radius, "Dx@Sketchx", If you move the curve over to the tooth (as the tooth is centered in Rolands example on the y axis) then the curve is no longer good. So ... I left it on the axis an proceeded to apply Roland's technique of mirroring the surface about a mirror plane AND added the Global Variables I wanted to be able to create a family of gears.
Now I am happy and I have attached the model here for all to use.
Very cool that you took the time to do this. Not sure where the error in the curve came in. Probably when it was moved and reconstrained.
In some versions, the involute is positioned by pressure angle at pitch diameter. In others, it is positioned by tangent at base diameter. I suspect the latter induces some position error, as the curvature at that location is rapidly approaching infinity as the curve approaches the base diameter.
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