Solved: Help with chamfer gear's

jambrozy

Hello Fusion guys!

I have problem with chamfer gears with 90° angle on drawing in attachment. Maybe someone can check this and give some concept?

Thank you in advance for your time.

Dawid.

HughesTooling

First some advice on your design. Move should be avoided as it's not parametric and joints are a better option.

So first, after creating the gear unground it so you can position it with a joint.

Next add a joint to position the gear. Like this any modifications to the design and the gear will stay in the correct position.

No need to create a sketch and extrude, you could just extrude a face or just use a combine cut.

Here just using a face and extruding.

See attached file.

I will make another post on some more suggestions and tips.

Mark Hughes
Owner, Hughes Tooling
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jambrozy

Thank you, I download file and check how you do that, I appreciate it very much 🙂

HughesTooling

First tips about the first sketch you created.

Seem odd not to use the document axis as the rotation axis for the part.

Also if you set the centre line type to centre line you can dimension using diameter sizes.

Edit Forgot to mention you set the line type on the sketch palette.

Here centre line moved to document origin and changed to a centreline and dimensioned using diameters also sketch is now fully constrained. Need to constrain the length on the centreline to make fully constrained.

Mark Hughes
Owner, Hughes Tooling
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HughesTooling

Next need to fix sketch6.

Personally I avoid symmetry constraints as they slow the sketch solver if there are too many.

This is my simplified version of the sketch using a pattern. Note the use of horizontal constraints rather than symmetry. Again, the sketch is now fully constrained.

Mark Hughes
Owner, Hughes Tooling
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HughesTooling

@jambrozy Attached is the file with all my changes.

Now what exactly do you need on the back of the tooth profile? A fillet like this?

Mark Hughes
Owner, Hughes Tooling
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HughesTooling

I see now there was an error in your first sketch. The hole should have been 67.5mm before cutting the gear profile.

So now with the correct profile in the rear is this what you want with a chamfer?

Mark Hughes
Owner, Hughes Tooling
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jambrozy

Thank you for all the tips. Right now, the most important thing for me is to correctly draw the teeth and perform chamfering next to detail C on the model. We have a width of 0.2 ... 0.4 mm that should remain after chamfering, and an angle of 90°. I'm just wondering if using the chamfer option from modify performs it according to the drawing (?)

HughesTooling

I'm really not sure what you're trying to achieve.

Is it a chamfer around the whole edge of the tooth like this. I think it will be easier to model one profile then pattern the profile with the chamfer.

This is what it looks like after patterning.

Mark Hughes
Owner, Hughes Tooling
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jambrozy

I work in the technology department as a CNC machine programmer, and according to our engineers, the chamfering should look like the one in the attachment. Unfortunately, I can't precisely achieve this with Fusion. Of course, we might be wrong. In my initial attempts, I also chamfered according to your idea, but the thinking here is different. Now, I don't know what to think about it anymore.

jambrozy

Can you add file which you created? I want to see this chamfers from your screens. I show tomorrow this my manager and we will see what he tell me ;o

HughesTooling

I've experimented a bit more but I think this is the same as the pictures above. Also please don't attach pictures, you can just paste them into the message or use the photo option.

Mark Hughes
Owner, Hughes Tooling
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HughesTooling

Here's another idea I think matches you pictures a bit better. See attached file.

Mark Hughes
Owner, Hughes Tooling
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MRWakefield

Aside from your chamfer issue that @HughesTooling has solved are you sure that the 'gear' profile (which I think should actually be an involute spline profile instead) is correct? English is my native language but I think the drawing states a between-roller measurement of 57.2+0.02+0.05mm where the roller dia is Ø4.01mm. I have sketched it up and the between-roller distance is 58.75 on your model.

Just thought I'd give you a heads-up in case it caused you issues down the line.

If this answers your question please mark the thread as solved as it can help others find solutions in the future.
Marcus Wakefield

___________________________________________________________________________________________________________
I've created a Windows application for creating custom thread files for Fusion. You can find out about it here. Hope you find it useful.
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HughesTooling

If I use Fusion's gear add in and create a gear with a 2.11666 module 30 teeth and 30° pressure angle I get something around 58.1. Can't get it exact because you can't use tangent constraints on a spline.

This shows the profile of the Fusion generated gear on top of the one in the file. Could increase the size by increasing the Module a small amount.

Mark Hughes
Owner, Hughes Tooling
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MRWakefield

Yes, I did a similar comparison to see if I could determine whether @jambrozy had done something similar to get the profile. I chose to use the Imperial (DP) version, but it would come out the same as the metric equivalent that you used in your example. My gear wasn't an exact match to the one in the model so just decided to mock up the measurement between rollers in a sketch. All I was ultimately trying to do was to check whether the design had the correct form as it didn't look right to me (and didn't seem to match the drawing) and was sure that a gear and a splined coupling with the same module(or DP) and pressure angle aren't the same. I didn't want the OP to manufacture to the model they provided without being absolutely sure it was correct.

If this answers your question please mark the thread as solved as it can help others find solutions in the future.
Marcus Wakefield

___________________________________________________________________________________________________________
I've created a Windows application for creating custom thread files for Fusion. You can find out about it here. Hope you find it useful.
___________________________________________________________________________________________________________

HughesTooling

Using the Fusion gear add in with this setting might work.

Also needed to adjust to OD of the gear to 68mm to match the part and came up looking like this.

I've attached the design for reference.

Mark Hughes
Owner, Hughes Tooling
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HughesTooling

@MRWakefield wrote:

I didn't want the OP to manufacture to the model they provided without being absolutely sure it was correct.

I guess it depends on if you just specify the sizes on the drawing and let the gear cutter get it right so the drawing only needs to be somewhere close?

Mark Hughes
Owner, Hughes Tooling
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MRWakefield

That's much closer but I think the addendum and dedendum will still need modifying to create the 'stubby' form required of a splined coupling. We're definitely getting closer though 😉

EDIT: Here's some info on calculating the correct values: https://www.engineersedge.com/gears/involute_spline_13649.htm

EDIT #2: This might also be useful: https://www.geartechnology.com/ext/resources/issues/0919x/spline-design.pdf

If this answers your question please mark the thread as solved as it can help others find solutions in the future.
Marcus Wakefield

___________________________________________________________________________________________________________
I've created a Windows application for creating custom thread files for Fusion. You can find out about it here. Hope you find it useful.
___________________________________________________________________________________________________________

HughesTooling

It really looks like the OD of the spline is less then the 68mm diameter behind the spline area so not sure using the gear is correct?

Mark Hughes
Owner, Hughes Tooling
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Help with chamfer gear's

Help with chamfer gear's

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