[cloverfield333]

in the bottom part of this picture:

http://www.outdoorebooks.com/ebay/webley/im-12.jpg

how does one go about making the ramp type ratchet (on the extractor) on a 3D extruded boss in solidworks?

any help would be appreciated...

[tobyaxis]

I am not an SW user but maybe a Loft Boss or Helical Boss would work.

Just a thought.

[cloverfield333]

how do you access the helical or loft boss on solidworks 2009?

and what exactly do they do.

[Beta]

By, "Ramp", Do you mean on an angle? The question doesn't seem very clear to me...

[Beta]

Or are you trying to protrude and rotate the sprocket a given distance?

[cloverfield333]

By, "Ramp", Do you mean on an angle? The question doesn't seem very clear to me...

Yes i would like to "cut" those angles/ramp out of a round excluded boss like the one i have attached here.

[userx]

This doesn't look to hard but I can't understand the geometry very well. Can you upload a larger image of the sketched section of the picture? I like a solidworks challenge!

[userx]

I took a quick shot at it. I am not sureI have captured the geuometry correctly but I think it will give you a start.

I created a helix, and a sketch containing a profile to sweep along the helix. I did a cut, sweep and this is what I got. Let me know if I am way off.

[allesg]

Are you trying to put a ramp on the side of a cylinder?

If so, do an extrude boss of a rectangle the right size placed on the cylinder where you want it, then from the side of the rectangle do an extrude cut of a triangle thru the rectangle to take away the material you don't want.

[cloverfield333]

thanks for your help. I saw the final product, but i am still not completely understanding how you made the ramps.

how does the cut sweep function work?

can you explain step by step how you were able to make these cuts?

[userx]

Sure,

start by creating a helix,

go to: insert - curve - helix/spiral

Select your round face as the sketch plane and draw a circle starting in the center and co-radial with the od of the sketch plane face. Accept the sketch with the check mark.

I chose to use "Pitch and Revolution" for the defining features of the helix. I don't know what the real pitch is based on the drawing you posted so I used .5in as a guess. I saw 6 ramps on your part, I know there is 360° in a circle and a small land just after the finish of the cut feature so (360°/6 ramps) minus a little gave me a revolution of .15. and I used a start angle of 0° to ensure the helix started on one of the default datum planes (easier for me to sketch on later). Accept the helix with the check mark. You will have a small section of a helix (.15 of a revolution to be exact).

Next choose the plane that intersects the begining of the helix and cuts your cylinder in half from the model tree and place another sketch on the plane. This will be sketch5 in the model I uploaded

Draw a rectangle from the OD of you cylinder (where the helix starts) and give it a height over the cylinder of .25. give the center hub a diametric dimention of whatever you want, I used .25in.

Now choose, Insert - Cut - Sweep

choose the rectangle you sketched, then choose the short section of helix. This is going to cut/sweep the rectangular section accross the helical path. Then I just patterened it 6 tiem around the part. Good luck, is that the geometry you were looking for?

[cloverfield333]

Sure,

start by creating a helix,

go to: insert - curve - helix/spiral

Select your round face as the sketch plane and draw a circle starting in the center and co-radial with the od of the sketch plane face. Accept the sketch with the check mark.

I chose to use "Pitch and Revolution" for the defining features of the helix. I don't know what the real pitch is based on the drawing you posted so I used .5in as a guess. I saw 6 ramps on your part, I know there is 360° in a circle and a small land just after the finish of the cut feature so (360°/6 ramps) minus a little gave me a revolution of .15. and I used a start angle of 0° to ensure the helix started on one of the default datum planes (easier for me to sketch on later). Accept the helix with the check mark. You will have a small section of a helix (.15 of a revolution to be exact).

Next choose the plane that intersects the begining of the helix and cuts your cylinder in half from the model tree and place another sketch on the plane. This will be sketch5 in the model I uploaded

Draw a rectangle from the OD of you cylinder (where the helix starts) and give it a height over the cylinder of .25. give the center hub a diametric dimention of whatever you want, I used .25in.

Now choose, Insert - Cut - Sweep

choose the rectangle you sketched, then choose the short section of helix. This is going to cut/sweep the rectangular section accross the helical path. Then I just patterened it 6 tiem around the part. Good luck, is that the geometry you were looking for?

when you say round face you mean the outer edge of the cylinder?

and the circle is sketched from the center or on the surface?

i am confused about this point.

[userx]

Not the outside edge but the flat face, just like you saw when you made your original extrusion. Sketch planes must be just that - a plane. you can't sketch on a cylinder wall. That being said; you can project a sketch onto a cylinder, and you can also create 3d sketches but neither of those things have anything to do with this lesson.

[userx]

Here is an image of the model showing the sketch plane, and the helix highlighted in green. You have not created the shown helix yet. If you expand the cut-sweep2 feature and expand the helix/spiral1 feature you will see sketch3. This is the sketch of the OD you are trying to create in order to generate a helix.

[cloverfield333]

okay now my problem is with the helix.

i can't get it togo around the surface.

i will send an attachment of what i did.

i don't understand what i am doing wrong.

[userx]

right click on the helix and edit this feature. Choose the check box that says reverse direction and change the revolutions to .15. You are almost there!

Another thing you should do is fully define your sketch5 (inside the helix). Make the diameter of your sketched circle the same as the diameter of your existing cylinder with a dimension or a constraint.

Now modify the sketch7 feature and delete the .425 dimension. drag the top of the rectangle down and completely off the cylinder. Then add a height dimension of .25 to define the rectangle. Choose the check mark, and try to create the cut/sweep feature.

Are you pretty new to solidworks?

I patterned it and added some radii...

[cloverfield333]

I created the rectangle but now i'm having problems with the cut-sweep option...

It isn't active when i go to the insert menu.

[cloverfield333]

okay, i now go the cut sweep to work, however not i'm having problems with the circular pattern function to make the other cut sweeps.

can you explain how to use the circular pattern because when i use it it does work?

[userx]

Sure but I am at home now and I don't have solidworks on this PC so I am going to do it by memory. Select the feature you want to pattern in the feature tree, then with it highlighted select the circular pattern icon. You want to pattern the feature 6 times, and it will want you to chose a direction so pick the edge of the circle. That should be it. Choose the check mark to finish. Have you done any of the tutorials that come with solidworks? You can access them in the help menu. Good luck!