Worm Gear

[mroy0404]

Hi Guys

 

 

I have drawn this worm gear and would like to machine it on a Doosan 2000sy with live tooling and y axis.   In mastercam what toolpath would be best using the live tooling with a 1/4" ballnose end mill.  Can a C axis tool path read from a solid model? I have tried using mill muti axis flow tool path with the best results, but the dam tool only wants to feed down one angle then back up the second angle, this causes way to much material for the cutter. could there be a tool path that would cut multi pass's for the width then step down to clear all the material first?

 

 

The gear is 5" dia  x 1.25 pitch. 

 

 

Any help would be great

[CJep]

You are probably going to get the best results with a multiaxis tpath locked to 4 axis.

In your multiaxis flow tpath were you using the pattern surface as the drive surface also?

[mroy0404]

Thanks for the reply CJep

 

I have the pattern surface applied,   the problem really is the tool wants to follow the surface down the surface than back up the second angle. this leaves way to much material for the endmill. Could there be a way to make the tool take depth cuts roughing out the worm in steps?

 

 

 

 

[Guest]

I've done a similar part to that and I used flow 5-axis and locked it to 4. I machined the floor first using the walls as check surfaces, then went down the walls for a semi-finish and finish using the floor as a check surface. IIRC that is. This was back in the V8 days... yeah... like 10-15 years ago.

 

That's totally doable though. You're gonna have crap ton of code, hope your machine is set to run off the memory card.

[CJep]

Without a part file there is really no way to dissect the tpath and offer solutions.

[Matthew Hajicek - Singularity]

I did something similar on a 4 axis mill back around '96 or so.  I couldn't find toolpaths I liked so I wrote a quickbasic program to generate the NC from the tooth profile points.  I also had to write a simple 4 axis backplotter to check my work.  Should be much easier nowdays.

[crazy^millman]

I would break it into section on that machine and approach it totally differently. With C axis you are really limited on what you can get away with for an effective toolpath. Natural shape limitations become the major thing working against you here. Yes it can be done, but I would do a peel mill in steps to rough the profile down in the V shape. Then I would come back with a custom made profile tool and try to cut the walls in one pass. Maybe taking .002 per pass till I achieved my required PD. Hobbing machines are best suited for cutting gears trying to make this on a CNC lathe will make something, but I would not think it will be correct.

 

Best of luck.

[HEAVY METAL]

I did something like this. i used a combination of flow 5x , curve 5x and morph between 2 curves. the last two to rough and finish land and flow 5 x to rough and finish sides. My land was a lot wider. Part was auger type screw.

[newbie70]

If it is a single start, try with Y-axis unroll method - 4 axis VMC.

I just designed a double start worm in MCX -solids. It needs trimming though.

[mroy0404]

Thanks for all the replies guys.

 

I ended up using a 1/4" ballnose end mill with 5 Axis flow toolpath locked to 4 axis and follow surface pattern for the cut parameter. What really helped was to extrud the tooth profile in sections (8 sections to be exact) this created 8 separate surfaces to control toolpaths and depth of cuts. I first created a roughing program leaving .100 on walls and .025 on floor.

The finishing program ran smoothly at 1 hr 30 minutes cycle time with about 18000 lines of code!

 

Thanks again for all your replies

[mroy0404]

Here are two of the 3 worms that the proper toolpaths produced.

[crazy^millman]

Here are two of the 3 worms that the proper toolpaths produced.

 

Good work. Run them through a couple times and you will polish up those faces in not time.