how to make serration groove

[Anonymous]

I have to make serration (circular groove) on the face of the flange. The problem each groove dia will be different or incremental to the previous groove. I don't want to draw sketch for each one, that will be too much work. Of course, pattern won't work either.

Any idea, please share! Below is the pic of it.

[danielw88]

I am not going to call this a perfect solution, and most likely as inadvisable as it uses the coil feature. Because the serration groove is so tiny, the amount of revolutions you would need to make to fill the entire surface would be large enough that it would present considerable lag on the system.

Make a sketch on a plane perpendicular to the disc's face. Draw a circle on the plane with a diameter of the groove. Place the circle close to the inside bore, ensuring that the circle is in the bore's area. Constrain the circle so that its center point is on the surface of the disc.

Select the coil feature. Select the circle that you drew for the profile and select the center axis of the disc as your feature axis. Under the coil size tab, select 'Spiral' as the type of coil and make the pitch 2x your groove diameter. Enter in the amount of revolutions that will completely cover your part's face.

Select 'OK', allow a few seconds to a bunch of seconds for your computer to process the part.

Once again, this isn't the most advisable method because it creates such a large feature, but if you NEED to do this, this is a method that i found worked. There may be other methods that i haven't thought of.

[JDMather]

Are you sure it isn't a spiral groove rather than concentric circular grooves?  (far less expensive to machine spiral and easier to model)

If it is spiral then use the Coil command and expand the drop-down selection for Coil Size>Type>Spiral

[hosford]

using the spirol command with a pitch similar to what is shown in your image will produce a part that is about 3 meg larger than one without the spirol, this wouldnt be so bad if it was just a part, but place a few of these in an assembly and you will wait for rebuilds.

[Anonymous]

it is concentric circular groove not spiral or phonographic, otherwise I would have used the coil command as other suggested.

[Anonymous]

I think for the modelling purpose and showing on the dwg, coil>spirol command does what is needed but file size goes too big..I hope there could be material style that can be applied such as expanded metal.

thanks for your input!

[Anonymous]

If done correctly using the spiral method, there is no way anyone would catch that it was done with a spiral method as oppose to a concentric method.  Unless it is absolutely vital that your part be modeled with the grooves in a concetric fashion, I say just go for the easy spiral method.  Otherwise, have fun with the concentric way

[Anonymous]

i would try something like this, create a sketch that crosses you part, project the edges, draw you grooves, if they decrease down at a specific rate, you can use a formula for dimensioning them down,

once sketch is done, use the revolve/cut command

PS-you dont say which version you are using, that attached part is 2014

Good Luck

[hosford]

sketch your groove cut then pattern it in the sketch, revolve using remove.