Need help in making a solidworks compatible file

I need help in generating the G-code to machine a gear like the one in the picture below. I would like to make a .dwg or .iges file of a gear (just the outer part as if the gear was solid in the middle) that i only have a picture of with no dimensions (other than the ones i'm choosing). The total diameter of the gear is 1.375", the root gear is 1.295" there are 72 teeth cut like a "V" and the length of each line that makes up the "V" is .050". I'm not very knowledgeable in CAD programs, and wondering someone here can help make a file that i can use in solidworks??? Thanks in advance for any help.

Hi Brian,

All you need to do is to draw the 2 defining circles as construction lines, 1.375 & 1.295 diameter, add a concentric relation and then dimension them both.

The next step is to draw some centre lines length 0.75 at various angles starting from the centre of the circles, the angles being 0, 2.5 and 5 degrees.

Now draw 4 lines connecting the following intersections :-

inner circle outer circle
0 degree 2.5 degree
5 degree 2.5 degree

The last step is to select Tools > Sketch Tools > Circular Pattern

the set # of instances to 72
angle A 360
and set equal spacing

with these settings make sure that the entities to pattern area is highlighted
and then select the 2 lines which make the first tooth and then press the OK button.

The 2 circles can then be deleted if required.

Hopefully this should do the trick, it worked with SolidWorks 2006


Dave

Sorry guys I edited Brian's post by accident... I think it's back to it's original form.

FWIW, machining these parts would not require drawing them just to get the G code. This is something which is easily programable just by hand writing the code. You need a 4 axis machine to machine the parts but you would regardless [whether you draw it and then use a CAM or just hand code it]

You'll need a tool which is ground to the shape of the tooth before you start, as well as the machining equipment.

The code in it's basic form is
F[set feed speed] S[set spindle speed]
G0 x0 y0 z [some dim larger than the major diameter]
G1 z [to minor diam of tooth]
x [width of tooth--this is the part that actually cuts the tooth]
G0 z [ move back up to clearance height ]
X0 A [360/# of teeth]

Repeat this times the # of teeth.

Voila..
J

Jerry,

The only thing different is the attached image.
Here's the same thing in another post.
http://www.cnczone.com/forums/showthread.php?t=57313

The ratchet is only a sample of what a gear looks like.
The numbers don't work out for the ratchet.


Brian,
For your gear, you will need a custom made V cutter, as said.
Yes, you can cut this on a vertical mill, manual or CNC.
Indexer or 4th Axis needed, also stated.

There are many ways to model your gear.
Are you using Solidworks? Are you a student?
I only ask because your others posts seem to indicate you are working on a project making gun parts.

pix

I'm not very knowledgeable in solidworks, though i do have solidworks 2007 on my computer. I'm just trying to make a ratchet like the one in the pictures i posted.

"FWIW, machining these parts would not require drawing them just to get the G code. This is something which is easily programable just by hand writing the code. You need a 4 axis machine to machine the parts but you would regardless [whether you draw it and then use a CAM or just hand code it]

You'll need a tool which is ground to the shape of the tooth before you start, as well as the machining equipment.

The code in it's basic form is
F[set feed speed] S[set spindle speed]
G0 x0 y0 z [some dim larger than the major diameter]
G1 z [to minor diam of tooth]
x [width of tooth--this is the part that actually cuts the tooth]
G0 z [ move back up to clearance height ]
X0 A [360/# of teeth]

Repeat this times the # of teeth."

Thank you.

Quote:

---

Originally Posted by brianklein

"FWIW, machining these parts would not require drawing them just to get the G code. This is something which is easily programable just by hand writing the code. You need a 4 axis machine to machine the parts but you would regardless [whether you draw it and then use a CAM or just hand code it]

You'll need a tool which is ground to the shape of the tooth before you start, as well as the machining equipment.

The code in it's basic form is
F[set feed speed] S[set spindle speed]
G0 x0 y0 z [some dim larger than the major diameter]
G1 z [to minor diam of tooth]
x [width of tooth--this is the part that actually cuts the tooth]
G0 z [ move back up to clearance height ]
X0 A [360/# of teeth]

Repeat this times the # of teeth."

Thank you.

---

Your diameter will really be 1.3724"

The included angle of your form cutter will be 76.35 degrees

Can be cut with a common 45 or 60 degree dovetail cutter, manual or CNC.

enat

Thanks for the diagram

"Your diameter will really be 1.3724"

The included angle of your form cutter will be 76.35 degrees

Can be cut with a common 45 or 60 degree dovetail cutter, manual or CNC."

How did you determine that the form cutter angle would have to be 76.35 degrees??? How can you get a 45 or 60 degree dovetail cutter to cut an angle 76.35 degrees??? And the total diameter (from tooth tip to opposite tooth tip) for the gear is 1.375" so how did you get 1.3724" for the diameter??? Thanks for your help.

Quote:

---

Originally Posted by brianklein

Thanks for the diagram

"Your diameter will really be 1.3724"

The included angle of your form cutter will be 76.35 degrees

Can be cut with a common 45 or 60 degree dovetail cutter, manual or CNC."

How did you determine that the form cutter angle would have to be 76.35 degrees??? How can you get a 45 or 60 degree dovetail cutter to cut an angle 76.35 degrees??? And the total diameter (from tooth tip to opposite tooth tip) for the gear is 1.375" so how did you get 1.3724" for the diameter??? Thanks for your help.

---

Brian,

I used your supplied data. I said in an earlier post your numbers don't work out precisely. I drew the model with your numbers and used Bamber's decription for sketching. Only I made a cut with the first V, then used a pattern feature to finish the full 360 degrees. With your numbers there is an overlap at the diameter, hence the slightly smaller diameter. I didn't include it, but the .050 lengths are a bit shorter too because of the overlap. This is due to using the 1.295 root number and the lengths of the V.

What does work out better is an angle of 74 degrees, this will give you the 1.375 diameter, with a small crest width of .0006, and the 1.295 root, but the flats will be .0493. By simply rounding the .0493 to .050, it changes everything.

Gear data usaually uses the pitch circle or diameter, where the gears engage, and a specific tooth form. The root and gear diameter will be nominal.

This is why I asked if you were a student, sometimes instructors will introduce a problem with nominal data to see how the student solves the problem.

As for the V tool. Yes you could have one made or grind one yourself and it might work okay in soft materials. But chances are the tip will break off while cutting unless you can get enough RPMs on it, like 10K+.

So I thought, if I had to make this today what would I use. And this is where the model really helps you, even a paper sketch. Look at the sketch, you can cut this off axis using a dovetail cutter.

In Solidworks I modeled the cutter, don't merge, and constrained it to the gear. This gave me the XYZA data using the face on the cutter. Then do the same thing and use the angle side of the cutter with the new XYZA data
and take the next pass.

Scott

Quote:

---

Originally Posted by pixburghenat

Brian,

I used your supplied data. I said in an earlier post your numbers don't work out precisely. I drew the model with your numbers and used Bamber's decription for sketching. Only I made a cut with the first V, then used a pattern feature to finish the full 360 degrees. With your numbers there is an overlap at the diameter, hence the slightly smaller diameter. I didn't include it, but the .050 lengths are a bit shorter too because of the overlap. This is due to using the 1.295 root number and the lengths of the V.

What does work out better is an angle of 74 degrees, this will give you the 1.375 diameter, with a small crest width of .0006, and the 1.295 root, but the flats will be .0493. By simply rounding the .0493 to .050, it changes everything.

Gear data usaually uses the pitch circle or diameter, where the gears engage, and a specific tooth form. The root and gear diameter will be nominal.

This is why I asked if you were a student, sometimes instructors will introduce a problem with nominal data to see how the student solves the problem.

As for the V tool. Yes you could have one made or grind one yourself and it might work okay in soft materials. But chances are the tip will break off while cutting unless you can get enough RPMs on it, like 10K+.

So I thought, if I had to make this today what would I use. And this is where the model really helps you, even a paper sketch. Look at the sketch, you can cut this off axis using a dovetail cutter.

In Solidworks I modeled the cutter, don't merge, and constrained it to the gear. This gave me the XYZA data using the face on the cutter. Then do the same thing and use the angle side of the cutter with the new XYZA data
and take the next pass.

Scott

---

Thanks again for the pictures!!! Now my question is while using the dovetail cuttters (are the yellow and blue cutters the same angle or two different ones?) how does one cut the V teeth with that cutter in the same pass??? And suppose i'm cutting the gear out of a rectangular piece of steel held in a vise??? how could i cut the teeth??? Thanks.

>>Thanks again for the pictures!!! Now my question is while using the >>dovetail cuttters (are the yellow and blue cutters the same angle or two >>different ones?) how does one cut the V teeth with that cutter in the >>same pass??? And suppose i'm cutting the gear out of a rectangular piece >>of steel held in a vise??? how could i cut the teeth??? Thanks.


Same cutter, same model, different color.

Two passes mininum. One using the face of the cutter, then one using the angled side of the cutter. You would have to reposition the tool.

Hold in a vise?.....are you are trying to make it more difficult?

Yes....if that's all you have, you sure could. You would have to make a fixture to hold and position the gear for each cut.

...and you could layout the teeth, remove excess material by drilling, then go at it with a 60 degree file. That's how it would have been done back in the 'olden days' ....

...and you didn't answer the question about being a student...are you?


pix

You could also do this on a watchmakers lathe...
I had a Schaublin lathe with an indexing plate, which with you could cut gears.

you can consider me a beginner at solidworks.

Brian,

What version of Solidworks do you have?

If you have at least 2007, I'll post a sketch to get you started and you can
mess around with the extrudes, cuts, and pattern.


pix

I do have Solidworks 2007. I have a .PDF file of another ratchet design. The ratchet OD diameter from the tip to tip of the teeth is a little above 1 7/32" (about 1.225") ,its groove to groove diameter is about 1.055" it is 7/16" thick and there are 18 teeth. You can see the picture of the ratchet in the .PDF that I have attached. Can you help me make a solidworks file of the Ratchet and if possible the pawl mechanism??? Thanks.

Quote:

---

Originally Posted by brianklein

I do have Solidworks 2007. I have a .PDF file of another ratchet design. The ratchet OD diameter from the tip to tip of the teeth is a little above 1 7/32" (about 1.225") ,its groove to groove diameter is about 1.055" it is 7/16" thick and there are 18 teeth. You can see the picture of the ratchet in the .PDF that I have attached. Can you help me make a solidworks file of the Ratchet and if possible the pawl mechanism??? Thanks.

---

...here ya go.

I'm still messing around with the mate to make it follow the gear, but it's enough to get you going.

pix

Thanks for the ratchet and pawl files!!!

Sure thing Brian.

The gear was modeled and patterned using the feature pattern.

The pawl uses all sketches, including a sketch pattern with some of the instances suppressed. You can see how sketches can sometimes be confusing. The .100 dimension is there to simply constrain the sketch and to take it beyond the outside diameter. That goes for some of the construction line endpoints, they were trimmed to merely put them someplace.

pix