Thread mill Toolpath

[RCT]

Hello to all! I'm a little new here, so Iwill start with a quick intro. I'm an 8 year CNC Machinist/Programmer (Mostly FANUC) out of SA, TX. I'm using X mr2. I was hoping someone can explain how the thread mill toolpath comes up with the Major diameter (ID thread) or Minor diameter (OD thread). The "Allowance (overcut)" under the thread mill tab, changes the output of this diameter.. but I'm not sure why, or if that is what I'm suppose to use. Any help would be great! Thanks

[Moldmaker74]

Hi RCT welcome to the forum.

 

I have only cut internal threads with X, but how it works is you have to select the outside diameter of the hole you want to thread. You may have to create an new circle equal to the thread you want to mill if you model only shows the minor diameter of the thread. .500 Dia for a 1/2-13 for example. The "Allowance (overcut)" you mentioned will allow you to adjust the fit of your threads as they will probably be too small the first time you cut them. Also I select a undefined tool and call out the outside diameter of my threadmill and use a good stream of coolant.

 

Hope this helps.

[HANARD]

I am also new .... I have found that if you select a circle Mastercam uses that diameter for the threads major diameter.

However if you select a point you can then use the “MAJOR THREAD DIAMETER” dialog box to specify the major diameter.

Be carful because I believe that selecting a circle will override the dialog box.

[Rick Damiani]

Selecing a circle will override the diameter on a threadmill toolpath, so don't do that.

 

MasterCAM dosn't come up with either diameter if you don't use a circle as input, and dosn't care about the thread shape, pitch diameter, or anything else. The reason it's asking for major dia (ID) or minor dia (OD) is because it ignores all the irrevelant (in terms of the toolpath) details like the shape of the thread form (which is controlled by the shape of the tool).

 

The output of a threadmill is a helical path. How many helixes you get depends on how many threads you need to cut (pitch X thread depth) and how many teeth the threadmill has (active teeth). MasterCAM takes the diameter of the threadmill tool and comps it to the major (ID) or minor (OD) dia becasue that's the only way that works for every threadform. The minor dia for an ID thread or the major dia for an OD thread will be whatever the shape of the threadmill leaves it, so no parameters are needed for that.

 

On the overcut - that allows you to adjust the fit of the thread, and is essentially a value added to the thread dia. If you want a particular fit, you'll either need to know what the allowance is for that fit or you'll need to look it up.

 

Lathe's threading toolpath uses a threadform calculator and allows you to specify a fit class, so if you can't find it out any other way, you can always add a lathe definition, start a lathe thread path, and use the thread calculator to figure out what you are looking for.

[RCT]

Thanks guys, this clears it up a bunch. Makes perfect sense. I was modifying someone elses toolpath, the selected geo must have been one of the models circles, which is why the OD and ID diameters where grayed out!