Cutter Comp on Thread Milling

[mtnflyr]

Is it possible to have a thread milling op start in the center of the hole using Perpendicular Entry? I'm having trouble getting the cut to start in the center of the hole. It keeps positioning off center even though I select "Start at center"

[David Colin]

I did it before... so i'd say yes.

Did you chain an arc center (not only a point) ?

[mtnflyr]

Yes, I chose arc center instead of point to get where I am. It seems the cut parameters ignore the Start at center when you select Perpendicular entry.

[David Colin]

However I already did it for sure (with V9.1)... I have no Mcam seat here but i'll try tomorrow.

[mtnflyr]

Thanks for looking into it David.

[Midwest]

Try Contour Ramp

[mtnflyr]

Midwest, that seems to work well if you cut from top to bottom. Have you been able to make this type of cut from bottom to top? I've tried several different settings with poor results.

[Jack Neelands™]

doesnt your thread milling in X2 work?

 

 

 

[mtnflyr]

Apparently it doesn’t work the same in X2 as it did in X. I made my cut the same as in your example, but it doesn’t give me a line for turning on comp. It just goes directly to a helix.

I don't know how to include snapshot or I'd show you.

[DavidB]

Chris,

Silly question but is your tool small enough in Diameter to achieve what you want?

[mtnflyr]

The tool is big enough to fit in the hole, barely. That's why I need it to start in the center of the hole.

I can get the thing to cut, but I have to hand whip the program to feed down the center of the hole then move to the comp on position to start the cut. Trying to learn a way to avoid this. I think it worked differently in MX.

[DavidB]

Make the entryexit arc smaller. Sounds like you can't fit the arc you have and a linear move for cutter comp.

[Jack Neelands™]

To up load a picture you need to find a site that will host it for you so that it remains here on the forum ...I use photobucket as well as alot of others on here

1. you will need to register and they will give you an account

 

2. To load a picture ----hit print screen on your keyboard

 

3. open up MS paint on you puter and click your mouse on the screen - then hit control V

 

4. you can add notes to the piture at this point with arrows and squiggly lines to better explain what you are trying to achieve here

 

5. Save the file as a jpeg or Bitmat...you will find that Jpegs are smaller in kb size and faster to load

 

6. Load the picture from the photobucket website to your folder and it will refresh itself once your picture is loaded on there.

 

7. From the photobucket weside you will find 3 files extensions at the bottom of your picture

copy the bottom one that says jpeg with all the characters in it ....and paste it into the reply form for Mastercam ...it should look somthing like

 

[Doug Gabbey]

I could never get this to work right and it was logged as a bug last April.

See below

Doug,

 

 

 

I’ve logged it as bug 20229. If you find any other problems let me know.

 

 

 

Mark B

 

Application Engineer

 

CNC Software, Inc

 

 

 

 

--------------------------------------------------------------------------------

 

From: Metalore Inc. [mailto:[email protected]]

Sent: Tuesday, April 18, 2006 3:33 PM

To: Mark Baker

Subject: Re: PERPENDICULAR ENTRY FROM CENTER IN THREAD MILLING

 

 

 

Mark,

 

I'm glad I made it clear.

 

I see what you have done and that works better but as you say it looks like a bug.

 

Can I get a bug report number so that I can track it?

 

Hope it gets fixed soon and thanks for taking a look at it.

 

Best regards,

 

Doug

 

----- Original Message -----

 

From: Mark Baker

 

To: Metalore Inc.

 

Sent: Tuesday, April 18, 2006 8:27 AM

 

Subject: RE: PERPENDICULAR ENTRY FROM CENTER IN THREAD MILLING

 

 

 

Doug,

 

 

 

I see what your trying to do. Its not the “arc entry” that’s giving you the trouble, it’s the angle that your trying to maintain. So by typing in “A0” and starting from the Bottom to Top the toolpath should go in at A0 and not A270 like in the current toolpath. It looks like I’ll have to write this up as a bug. I think I have a work around, with the “helix entry” turned on and an “A90” value entered (should be A0), isn’t that giving you the toolpath that your looking for? We’ll be getting an “helical entry” move but its at the same pitch so the only thing that is wrong in the entry angle.

 

 

 

I’ll go ahead and log this as a bug.

 

 

 

Mark B

 

Application Engineer

 

CNC Software

 

 

 

 

--------------------------------------------------------------------------------

 

From: Metalore Inc. [mailto:[email protected]]

Sent: Tuesday, April 18, 2006 9:12 AM

To: Applications Inbox

Subject: Re: PERPENDICULAR ENTRY FROM CENTER IN THREAD MILLING

 

 

 

Mark

 

I am trying to make a straight line entry from the center of the arc to the start of the circle (A0) WITHOUT an on and off arc OR AN ON OR OFF HELIX and the same at the exit.

 

At the end I want it to go to the center without any arc or helix moves.

 

You have helical entry and exit set so you don't get arcs, you get helical moves.

 

If you turn off helical entry and exit you will see the 90 deg arcs I am talking about.

 

There is an option for perpendicular entry, I thought it would generate what I described in the first line but I still get arcs at the entry and exit.

 

If you want to phone me my number is: XXX-XXX-XXX or if you send your phone number I can call you.

 

Regards,

 

Doug Gabbey

[mtnflyr]

OK, well I guess I can stop banging my head on the keyboard now. It's a bug. Thanks for the info Doug.

 

Jack, thanks for the snapshot info. That will come in handy.

[jeff]

If your entry/exit arc clearance is too large, it should start at the center of the hole.

Try making this value a large one and see what happens.

[Qmp]

Chris

 

We do alot of thread mill here, With X2 So far we don't have any problems yet. What size of thread hole you want to mill and tool Dia ? Let me know I will take a look.

 

Qmp

[mtnflyr]

quote:

---

If your entry/exit arc clearance is too large, it should start at the center of the hole.

Try making this value a large one and see what happens.

---

Jeff, this is the setting I've been missing.

It was set at .1, too large for this application. I'm milling a 1/2-13 hole with a .420 dia. thread mill. The same size as the minor dia. I set the entry/exit to 0.0 and it works perfectly now.

 

Thanks for all your help everybody.