pitch when threading

[k_barry]

How can I output the pitch when I am using a threading cycle. I use Mill v9 and very new to it.

 

Secondly, I cannot understand the method that Mastercam outputs feedrate.

I use mm units and want mm/rev rather than mm/min.

Does anyone know of any good text or reference books on posts, that tell me the names of some of these variables?

The manuals I got with Mastercam are only tutorials and have nothing in it.

I have hard coded the mm/rev G function into the begining of the post but I do not know where the feedrate comes from.

[John_o]

Toolpaths-next menu-Circ tlpths-Thread mill

Hope this helps mate.

Its new to me as well, I skipped V8

[kccadcam]

Mcam always figures mm/min, to change this you need to add something like this in your post:

"feed = (1 / n_tap_thds)" (change to metric obviously)

under the ptap function.

Have your dealer come and help you out.

 

[ 08-27-2002, 03:46 PM: Message edited by: Kevin Clark, Central Valley Machine ]

[PE @ IHS]

It seems to me that you are talking about tapping cycles, rather than threading cycles (as in a lathe). The two replies above are in reference to the threadmilling feature in Mastercam.

 

If it is tapping that you are referring to, the solution is easy. Please clarify.

 

Peter Eigler

[Jack Mitchell]

k_barry,

 

Assuming you a tapping on a machining center.

 

I will attempt to clartify in imperial or inches. - please don't be offended, this is by no means my intent.

Using a 1/2-13-2B UNC Tap

( 1/2 refers to the nominal thread diameter)

( 13 refers to the number threads per inch)

( 2 is class of fit & B for internal thread)

(UNC refers to Unified National Course - an American standard 60degree thread form)

 

When using G95 (inches per rev or mm per rev)

G43 H03 X0 Y0 Z2.0 S1000 M03 M08

G98 G84 X0 Y0 Z-.5 R.1 F.0769

X1.0

G80 G49 Z2.0 M09

In this example we program the actual tap pitch.

 

When using G94 (inches per min or mm per min)

G43 H03 X0 Y0 Z2.0 S1000 M03 M08

G98 G84 X0 Y0 Z-.5 R.1 F76.92

X1.0

G80 G49 Z2.0 M09

In this example we multiply program the tap pitch by the actual rpm.

 

I personally prefer programming to utilize G95 - I need to better educate myself about feeds, speeds, chiploads etc!

When we utilize G94 - I need to better educate myself about feeds, speeds, chiploads etc! AND THEN MULTIPLY this by the rpm.

Mastercam will calculate your feeds in mm per min based on your thread pitch times your rpm.

 

Regards, Jack

[k_barry]

Thanks, I tried the thread mill and it just outputs about 500 lines of code in small straight lines.

 

About my dealer.... I bought Mcam in june and have one mill and one lathe. I got about 6 hours training. I have received the mill post but am still waiting on our lathe post.

I have got more info from this forum.

I keep going back to my old CAM system instead of Mcam.

Mcam seems a good program but different to what I am used to and I cannot find the time to fiddle.

I am modifying too much cnc code in the editor.

 

Thanks for the replies

[k_barry]

I was replying while there were 2 other replies coming in... May look a bit confusing.

 

I am Tapping (G84) in a vertical MC - Okuma.

I also like feeding in units/rev rather than units/min.

Thanks for the replies

[PE @ IHS]

I was mistaken, since you are, in fact, talking about threadmilling, not tapping.

 

Which control is it? Are you looking for a canned cycle output for threadmilling, or at least G02-G03 interpolation? This can be easily done by turning your arc filter on. Some post mods may be needed if you want to output entire circles instead of quadrants. We can help more if we know the control as well as the expected result.

 

During threadmilling, your output should be G02 or G03 with a Z motion equal to the thread lead on the same line (pitch and lead are not the same thing)

 

Don't give up on your Mastercam and don't be shy to ask the folks here for help

 

Peter Eigler

 

[ 08-27-2002, 07:48 PM: Message edited by: Peter E ]

[kccadcam]

Peter,

I was referring to tapping not threadmilling.

Jack,

Putting that formula into ptap in your post calculates the proper feed for inches per rev because like I said Mcam always figures inches per minute when you define a tap.

[PE @ IHS]

Hi Kevin

 

I realize you were talking about tapping, but apparently the original question relates to threadmilling. The output FEED in threadmilling is irrelevant to thread accuracy. The thread lead is determined by the amount of Z axis movement for each complete circular pass, not the feedrate. The feedrate increased or decreased based on tooling and fixturing needs and the thread will still come out correct.

 

Peter Eigler

[kccadcam]

quote:

---

I am Tapping (G84) in a vertical MC - Okuma.

I also like feeding in units/rev rather than units/min.

---

I think the original post was about tapping.

[kccadcam]

This is how I set up my Matsuura with rigid tapping:

code:

---

 pmisc2          #Yasnac Rigid Tap

pdrlcommonb

pbld, n, "G93", "(RIGID TAP)", e

feed = 1 / n_tap_thds

pcan1, pbld, n, *sgdrlref, *sgdrill, pxout, pyout, pfzout, pcout,

prdrlout, *feed, strcantext, *speed, e

pcom_movea

---

And this is how I cancel it:

code:

---

 pcancelrig       #Cancel Yasnac rigid tapping cycle

result = newfs (three, zinc)

z = initht

if cuttype = one, prv_zia = initht + (rotdia/two)

else, prv_zia = initht

pxyzcout

!zabs, !zinc

prv_gcode = zero

pbld, n, "G80", e

pbld, n, "G94", e

---

 

[ 08-28-2002, 10:42 AM: Message edited by: Kevin Clark, Central Valley Machine ]

[gstephens]

Since you're dealing with metric taps, the value in the tool parameter page is going to make all the difference. For a matric tap, the box is for "pitch", whereas on an english tap the value is "threads" [per inch]. This causes a HUGE problem when posting because the value is sent to the post under the n_tap_thds varible no matter what units are being used. So for metric taps your feedrate should be something like:

 

feed=n_tap_thds

 

to get mm/rev for your output.

Make sure you add the appropriate G-code to switch to mm/rev (unless the G84 does it automatically).

[PE @ IHS]

Hi Kevin

 

Perhaps I am still asleep, but the FIRST post was about threadmilling, then halfway through it changed to tapping...oh well...I am just a dumb sales guy....I will stick to handing out business cards and looking pretty!

 

Peter Eigler

[kccadcam]

Thanks for for the info gstephens.

I don't deal with metric much so I didn't realize

that they are defined differently.

 

I guess my bum IS falling off!!

[k_barry]

Thanks gstephens

 

I will try this tomorrow and see how it goes.

Sounds easy.

Bit busy today...

Many thanks all

[k_barry]

Thanks all.. it worked well.

I can now move on to my next refinement.

Thanks