Drawing a saw blade – help!

[SillyOldDufferModerator @sillyoldduffer]

I learn CAD by tackling ever more difficult objects, mostly successful, but the latest has me stumped. My nemesis is a hole saw:

First attempt was easy enough, not worrying about the exact scale, below was done by creating a plane tangent to the cylinder, sketching a tooth on the plane, cutting through the cylinder with the sketch, and then replicating the cut with a circular pattern:

There are three problems!

First, the teeth don't align properly with the central axis. The error is more obvious on a small diameter hole saw and is caused by a flat sketch being projected parallel on to the curve.

Second, the teeth need to be alternately bent a couple of degrees in and out to create the kerf. Something like this, but easier to draw and replicate in a circle with properly shaped teeth;

Thirdly, the teeth in the real saw aren't all the same depth. It can just be seen in the first photo that the teeth nearest and furthest from the camera are deep and those to the side are shallow. Might be a manufacturing error except it looks neatly deliberate.

I don't know how to model this saw in CAD! I've failed with FreeCAD and Solid Edge in both Part Design and sheet-metal modes. Very grateful for any suggestions please!

Thanks in anticipation,

Dave

[SillyOldDufferModerator @sillyoldduffer]

[Anonymous]

Use a loft from the sketch to a point on the rotational axis to create the tooth shape?

Andrew

PS: In reality I expect the teeth are cut straight during manfacture with no taper

Edited By Andrew Johnston on 27/08/2022 22:43:57

[HuubParticipant @huub]

Posted by SillyOldDuffer on 27/08/2022 21:56:08:There are three problems!

The teeth don't align properly with the central axis. The error is more obvious on a small diameter hole saw and is caused by a flat sketch being projected parallel on to the curve.

I use Freecad and it takes some time to get used to it.

You need to draw a construction line from the centre of the saw blade to the cutting edge. Than you can set the angle between the cutting edge and this construction line.

You draw 1 tooth and use the polar pattern to draw all other teeth.

To bent 2 teeth, you draw 2 teeth and project the sketch on a curved surface. You can use the Curves workbench for this. Curve workbench

If you want to change the height of the teeth, drawing a bunch of teeth at the right height, projecting them on a curved surface and than making a polar array is an option. I can't think of an easier way at the moment.

To make life easier, you need to set all dimensions in a spreadsheet. The dimensions in the drawing can than be changed by just changing the dimension in the spreadsheet.

In the spreadsheet you can make a configuration table having different dimensions for different saw blades. You can then check your design changes for different saw blades by just selecting the right saw blade.

If any of these techniques is unknown, use Youtube to learn it.

[lee websterParticipant @leewebster72680]

Could you draw the tooth as a separate body, shape it so that it has the correct angles and then make a mirror copy in the correct axis moved the correct distance from the first tooth and cut both of the teeth bodies from the cylinder body then replicate the cut around the cylinder central axis. I think I made it sound more complicated than it is.

As for the cutter in the first photo, I have never seen a hole saw like that.

[Paul LousickParticipant @paullousick59116]

Hole saws like the one shown are fitted to a spindle and use a twist drill to centre the hole. Available at bigger hardware stores. They can be used on wood and sheet metal.

Dave, Another feature for you to incorporate is that the teeth ate set to give clearance for the saw. One tooth is bent out and the next tooth bent in. (The final grind appears to be in line with the drill centre)

Paul.

[JasonBModerator @jasonb]

Does the CAD that you are using have sheet metal? you may be able to draw it flat and then roll it up just like the saws are made.

If not you may be able to wrap the sketch of the teeth around the circle

The better makes of holesaw have the variable pitch to reduce chatter and noise, if you look on larger dia saws you can see it quite clearly. Also you get the odd part tooth where the rolled up blade is joined which confirms the teeth are cut then rolled

Is it just me that thinks Dave has too much time on his hands

 

Edited By JasonB on 28/08/2022 07:28:33

[Paul LousickParticipant @paullousick59116]

Nothing better than a good challenge if you have plenty of time on your hands to get the brain cells working. I started to model the hole saw but ran out of it !. Maybe later when I find some.

[Michael GilliganParticipant @michaelgilligan61133]

I’ve just logged-in for the first time in a while … and seen this interesting thread:

It immediately reminded me of a question I asked, back in 2015 …

MichaelG.

.

https://www.model-engineer.co.uk/forums/postings.asp?th=112241

Edited By Michael Gilligan on 28/08/2022 09:10:44

[JasonBModerator @jasonb]

I was only thinking the other day if you were OK Michael as you had been a bit quiet, I too was reminded of those images I posted some time ago.

[old martParticipant @oldmart]

It is not uncommon for saw blades to have variable pitch which could complicate things.

[SillyOldDufferModerator @sillyoldduffer]

Posted by Andrew Johnston on 27/08/2022 22:42:16:

Use a loft from the sketch to a point on the rotational axis to create the tooth shape?

Andrew

PS: In reality I expect the teeth are cut straight during manfacture with no taper

This suggestion works, or at least is a considerable improvement. Thanks!

Having a busy day so to save time the example is with a V tooth. First picture shows the sketch on it's tangent plane, lofted solid to a point on the axis, to show it's shape (Discovery: Solid Edge won't loft to a line.)

The same loft applied as a cut:

And the tooth with some chamfering rotated as a pattern cut around the Z axis:

Progress, but the tooth relief isn't quite right, and there's no kerf (teeth bent alternately) or variable depthing.

Jason suggested the Sheet-metal workbench, which I've tried. As far as I can see FreeCAD and SE don't allow a bend to be applied to a curved strip. It is possible to kerf the teeth on a straight strip, but I can't find a way of bending a straight strip into a circle.

Normally I find it easier to 3D-model in CAD than to make the real thing. This seems to be an exception: bending strip metal into a circle and kerfing saw-teeth is easy in real life!

Back to the drawing board!

Ta,

Dave

[JasonBModerator @jasonb]

I wonder if you could make it by combining two sketched. Draw as you have above but with a slight trumpet shape and cut the teeth plus a gap which will gibe you the teeth bent outwards. Then do an additional ring around the top that bends in slightly and cut the alternate teeth from that. When the two are combined you will have teeth set in either direction.

[Ed DuffnerParticipant @edduffner79357]

Can you select a set of points which form the profile of a tooth and move/rotate the those points in or out of the arc of the blade face?

[JasonBModerator @jasonb]

Needs a bit more work getting the inner and outer teeth the same size but basically what I said in the previous post using Boolean unite to make the flaired out tube and ring of flaired in teeth into one unit

Edited By JasonB on 28/08/2022 18:56:27

[SillyOldDufferModerator @sillyoldduffer]

SolidEdge Sheetmetal achieved this on a straight blade:

Hard work though because the teeth have to be bent one at a time – takes forever. Also the round holes are essential to relieve the bends: seems SoildEdge won't apply bends that break the rules!

A quick try with Ed's suggestion didn't work in Solid Edge (Sheetmetal) and I'll try in Part mode later.

I like Jason's trumpet idea, pretty sure SE can do the same and will try after I've eaten.

Cheers,

Dave

[Gary WoodingParticipant @garywooding25363]

Here's my effort in Fusion.

[SillyOldDufferModerator @sillyoldduffer]

This my first attempt at Jason's Trumpet method, proof of concept, with no attempt at getting the tooth details right. However it works, and is quick!

I'm impressed by Gary's Fusion360 version. How was it done?

Ta

Dave

[Gary WoodingParticipant @garywooding25363]

I first created sketch of two versions of the profile of the blade; one with the lip curving out and the other with the lip curving in.

Then each profile was revolved to create two bodies in the same location. Here's the one for the top sloping out.

A new sketch was then drawn from the top. This was to get the correct angle for the pairs of teeth – I chose 10 pairs.

I then created a workplane offset from the original sketch, but through the line defining the angle of the previous sketch.

I then cut then created a workplane to cut the two bodies along the horizontal line of that sketch. This created 4 bodies: two copies of the cylindrical parts, and one each of the in/out sloping parts.

[Gary WoodingParticipant @garywooding25363]

Continued…

I then lofted the two teeth towards the small rectangle in the centre.

Because the in/out sloping parts were now separate from the two cylindrical parts I could create an intersection of one tooth and the in-slope section, and the other with the out-slope section.

I could then do a circular pattern of the two teeth and then combine then with one of the cylindrical parts. That completed the job.

[HOWARDTParticipant @howardt]

Having followed this topic with the thought that the profile was wrong looked at manufacturing process. The saws are actually made from flat saw profile welded into a circle. Much easier to draw and get the correct tooth profile.

[SillyOldDufferModerator @sillyoldduffer]

Many thanks to Gary for his comprehensive description of how to kerf teeth on a hole saw with Fusion360. My next job is to replicate it in SolidEdge. (Almost certain the method will work, but I'm finding SE harder to drive than Fusion.)

Made progress on the third problem which is getting a pattern repeated cut to follow a wavy line projected on to a cylinder. This example punches a series of holes up, down and around a cylinder, and in principle it should work with teeth profiles:

Huub's suggestion of FreeCAD's Curves Workbench is on my To Do list, and I agree with him that planning with a spreadsheet is a good idea. The teeth don't line up in my attempts because I winged the dimensions rather than doing the sums.

I've already had a go at Howard's suggestion but – so far – not found a way in SolidEdge of bending a straight strip with teeth into a circle. I'm going to try again this morning. Feels like something the tool should be able to do.

Thanks to all

Dave

[SillyOldDufferModerator @sillyoldduffer]

Re Howard's suggestion – drawing the teeth on a straight strip and then rolling it into a circle. Turns out to be possible with SolidEdge Sheet-metal but not as I expected!

The trick is to:

1. Draw a circle with a break in it.
2. Extrude the circle with 'Flange Extend' to create a cylinder (with break)
3. Unbend the cylinder (a button) , producing the flat strip needed to make it
4. Add teeth to the flat strip
5. Rebend to put the flat strip back into circular form. (another button)

Image shows the Rebend action just before confirmation:

Dunno what's going on today, people keep me ringing up and banging on the door. Feels like family, friends and Postie have organised themselves to cause maximum disruption.

Dave

[JasonBModerator @jasonb]

That was my first suggestion too, to draw it flat and roll it up like they are made.

Can rolling it up include the set of the teeth?

[SillyOldDufferModerator @sillyoldduffer]

Posted by JasonB on 30/08/2022 16:27:52:

…

Can rolling it up include the set of the teeth?

Seems not! So close and yet so far…

Back to the drawing board!

Dave

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