5th Axis Mill Toolpath for ID Buttress Thread? (Reverse Angle Square Thread)

[Scott Chordas]

Working on getting a pool of information around for being able to do a Buttress Thread in a 5th Axis mill using Mastercam 2020. I know it can be done but I personally haven't done it yet. I am hoping to educate myself on the matter so I know my constraints and limits when setting up the toolpath. I have listed the thread and tool called out that would be used. I know the toolpath used cutter comp to control the size of the major diameter of this particular thread. This leads me to believe that the toolpath used was "Curve". I believe the toolpath has to be derived from a helix spiral geometry. Could anyone bring light to this toolpath?  

[JParis]

I would say it's most likely NOT a 5axis path...generally a 5 axis comp move can't be done(with exceptions)

That said, it's most likely it was a rolled toolpath which could be comped..

No file, no real idea what was or wasn't done previously

[Scott Chordas]

JParis, 

Would you be able to put more emphasis on a "rolled" toolpath? 

[JParis]

Yup..

Would you be able to share a file?

[gcode]

I have done this on our Okuma VTM 1200 using form wheel cutters and a 5 axis swarf toolpath 

I did not try using CDC, I just programmed to the nominal thread forum and cut it .

Doing it on a 5X mill the same way would not be a problem as log as the rotary axis had unlimited 360° motion

I've also done OD threads  on a 5X mill using endmills and swarf toolpaths

 

 

[Scott Chordas]

I can give you a x.t file of the thread but not the whole part. m9x1.25 minor 7.72mm major 9.205.X_T

[crazy^millman]

I would do a standard Threadmill and call it a day. No need for any 5 Axis toolpath here just call out the correct tool and run it.

[#Rekd™]

53 minutes ago, Scott Chordas said:

I can give you a x.t file of the thread but not the whole part.

Hi Scott,

Open that X_T file and save it as a Mastercam file. Then post the Mastercam file. 

[JParis]

I didn't get a a chance yesterday to look at this...being my last day before leaving on a short vacation, the demands on me were high...

Observation from quickly looking at it...I agree with crazy^millman...threadmill it and be done..

I glanced over the topic title, missing the ID....with a .354" ID doesn't seem to me that you can do much more....

 

[Scott Chordas]

Thank you

I got it to work by drawing geometry of a helix at a major dia of 9.205 with a pitch of 1.25mm. I then drew up the form cutter off of the drawing and linking it into mastercam by a "level". I used "curve" multiaxis toolpath. See image below for cut pattern but to sum it up curve type is the helix and radial offset is the tools radius (at smallest dia at 5° angle). For Tool Axis control see image below as well. The tool is set to rotate around the "Z" axis. Side tilt angle was set to 5.0 for the 5.0 degrees that cut into the tool. Lead/lag angle is set to -2.7743 because of the compound angle to allow for the tool to cut proper. 

Best of luck!

 

 

[crazy^millman]

56 minutes ago, Scott Chordas said:

Thank you

I got it to work by drawing geometry of a helix at a major dia of 9.205 with a pitch of 1.25mm. I then drew up the form cutter off of the drawing and linking it into mastercam by a "level". I used "curve" multiaxis toolpath. See image below for cut pattern but to sum it up curve type is the helix and radial offset is the tools radius (at smallest dia at 5° angle). For Tool Axis control see image below as well. The tool is set to rotate around the "Z" axis. Side tilt angle was set to 5.0 for the 5.0 degrees that cut into the tool. Lead/lag angle is set to -2.7743 because of the compound angle to allow for the tool to cut proper. 

Best of luck!

 

 

There was the missing piece of the process the tool drawing. You are trying to use a tool not designed to cut the thread and cut the thread with it. You needed to cheat the thread in. Congratulations that you were able to cheat it in and get it to work.

I am always trying to improve my way to help customers. If a customer asked me to do what was asked in this thread and forgot to provide me with the tool they wanted to use that they had a drawing for I would be hard pressed to come up with a solution like was asked here. Just curious how you thought anyone was going to be able to help sort that out without providing that key price of information?

[Scott Chordas]

Crazy Millman,

I am sympathetic to your remark about "not having what you needed". This is the very first post I have done on the Mastercam forum. I learned you can't use drag and drop when inserting a image into the text area. You must choose file then insert the file into the text area. I did not know at the time that my images did not get attached. Until you pointed out that there was no image of the form cutter. If you don't reach out to your customer asking if they have a specific tool then they might figure that is on you to come up with the tool to use. 

 

Scott  

[crazy^millman]

20 minutes ago, Scott Chordas said:

Crazy Millman,

I am sympathetic to your remark about "not having what you needed". This is the very first post I have done on the Mastercam forum. I learned you can't use drag and drop when inserting a image into the text area. You must choose file then insert the file into the text area. I did not know at the time that my images did not get attached. Until you pointed out that there was no image of the form cutter. If you don't reach out to your customer asking if they have a specific tool then they might figure that is on you to come up with the tool to use. 

 

Scott  

It use to be a lot easier added pictures and screen shots to the forum. We also could make links and do this crazy things like using emojis, but those days are gone and we have what we have.

Yes I normally call out the tools when a customer doesn't have anything to use.

[cncappsjames]

Just a technical note (machine side) to effectively use cutter comp on something like that, you'll need 3D Tool Comp G41.2/G42.2 and TCP G45.5 (IIRC) .. and a post that supports that..