Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

1 npt threadmill

JOHNAKA

By JOHNAKA,
in Industrial Forum

 Share

Recommended Posts

JOHNAKA Newbie

JOHNAKA

Posted
Posted

Hi,

 

need some help on threadmilling 1 npt in mcx6. I predrill the hole to 1.156 straight hole no taper wall. i have a threadmilling tool have defined it in custom level

12 thread of engagment to 1.125 long .087 picth thread and 60 deg. the tip dia is .554 the end taper dia is .620 . select the thread mill contour on the 1.156 circle and it gray out the pitch dia.

.087 pitch

stragt thread angle 30

.012 allowance

taper wall -1.783( wont come close to the wall until i put - 1.783 angle)

compensation type (computer)

id thread

right hand thread

from bottom to top

multi passes 3 (.02)

thread depth -1.043 to get full teeth engagement.

 

( i ran the code and so far i only get one turn on the gage.) what im i doing wrong .? help me please

one other things how i can make it post out the code as arc out instead of linears long codes.

 

sincerly

john

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Sounds like you just need to comp it out to get the gage to go to depth. This is not uncommon as I always have to comp out my threadmilling programs to accept the gage.

 

+1 to having to "comp" it out.

 

Threadmill tools can vary widely in actual profile shape. Look at "Allowance (overcut)" on the Cut Parameters page. This will allow you to enter a + or - value to adjust the toolpath. You mentioned you were using "Computer" for the compensation type. This means you don't get any cutter compensation on the machine, so this is where you will have to enter your increase in compensation to make the threadmill cutter bigger.

 

The other thing you could do would be to use "Wear" compensation, and adjust the wear register on the control until the gage will fit.

Link to comment
Share on other sites
K2csq7 Newbie

K2csq7

Posted
Posted

+1 to wear comp.

 

 

On the question of outputting arcs instead of lines...

Goto-

settings

machine def manager

control def manager (icon at the top that looks like a machine control with a red & green button)

arc (branch on tree of control def manager)

 

ensure "helix support" is set correctly (i.e. all planes supported for me)

Save with the icon at the top (saving control def)

green check out

Save with the icon at the top (saving machine def)

green check out

select yes to save changes and yes to replace machine group.

 

HTH!

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

i comp it out to .037 and it work beautifull, as for the arcs i will try this now, I apreciate All the help thanks

 

Sincerly

John

peace out

 

You are welcome John. Keep in mind that if you change the tool, you will have to adjust that compensation (allowance) amount in your program. That is the advantage of doing it using cutter compensation at the machine, you can adjust the compensation value there instead of having to repost the program again...

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

When threadmilling a taper thread its not cutting a true arc. As you go up in Z the arc gets bigger and bigger. I dont think you can get Mastercam to output arcs for this. At least I've never seen it.

 

There is somewhat of an exception here. While it is true that you can't do a tapered thread path as a series of 360 degree arcs, you can cut it as a series of 180 degree arcs where the center/endpoint of each arc changes.

 

Here is some sample output (I just threw in some numbers, .05 pitch, 4 degree taper)

 

G20

G0 G17 G40 G49 G80 G90

G0 G28 G91 Z0.

( 1/2 FLAT ENDMILL |TOOL - 1|DIA. OFF. - 239|LEN. - 239|TOOL DIA. - .5)

M11

M13

T1 M6

G0 G54 G90 X-4.2564 Y.424 B0. A0. S1069 M3

M10

M12

G43 H239 Z.25

Z.1

G1 Z-.5 F6.42

Y.3081

G3 X-4.0405 Y.424 Z-.4875 I.0769 J.1159

X-4.474 Z-.4625 I-.2168

X-4.037 Z-.4375 I.2185

X-4.4775 Z-.4125 I-.2203

X-4.0335 Z-.3875 I.222

X-4.481 Z-.3625 I-.2238

X-4.03 Z-.3375 I.2255

X-4.4845 Z-.3125 I-.2273

X-4.0265 Z-.2875 I.229

X-4.488 Z-.2625 I-.2308

X-4.023 Z-.2375 I.2325

X-4.4915 Z-.2125 I-.2343

X-4.0195 Z-.1875 I.236

X-4.495 Z-.1625 I-.2378

X-4.016 Z-.1375 I.2395

X-4.4985 Z-.1125 I-.2413

X-4.0125 Z-.0875 I.243

X-4.502 Z-.0625 I-.2448

X-4.009 Z-.0375 I.2465

X-4.5055 Z-.0125 I-.2483

X-4.2564 Y.174 Z0. I.2496 J-.0004

X-4.1064 Y.424 Z.0125 J.17

G1 X-4.2564

G0 Z.1

Z.25

M5

G0 G28 G91 Z0.

M30

%

Link to comment
Share on other sites
slyym Newbie

slyym

Posted
Posted

There is somewhat of an exception here. While it is true that you can't do a tapered thread path as a series of 360 degree arcs, you can cut it as a series of 180 degree arcs where the center/endpoint of each arc changes.

 

Here is some sample output (I just threw in some numbers, .05 pitch, 4 degree taper)

 

G20

G0 G17 G40 G49 G80 G90

G0 G28 G91 Z0.

( 1/2 FLAT ENDMILL |TOOL - 1|DIA. OFF. - 239|LEN. - 239|TOOL DIA. - .5)

M11

M13

T1 M6

G0 G54 G90 X-4.2564 Y.424 B0. A0. S1069 M3

M10

M12

G43 H239 Z.25

Z.1

G1 Z-.5 F6.42

Y.3081

G3 X-4.0405 Y.424 Z-.4875 I.0769 J.1159

X-4.474 Z-.4625 I-.2168

X-4.037 Z-.4375 I.2185

X-4.4775 Z-.4125 I-.2203

X-4.0335 Z-.3875 I.222

X-4.481 Z-.3625 I-.2238

X-4.03 Z-.3375 I.2255

X-4.4845 Z-.3125 I-.2273

X-4.0265 Z-.2875 I.229

X-4.488 Z-.2625 I-.2308

X-4.023 Z-.2375 I.2325

X-4.4915 Z-.2125 I-.2343

X-4.0195 Z-.1875 I.236

X-4.495 Z-.1625 I-.2378

X-4.016 Z-.1375 I.2395

X-4.4985 Z-.1125 I-.2413

X-4.0125 Z-.0875 I.243

X-4.502 Z-.0625 I-.2448

X-4.009 Z-.0375 I.2465

X-4.5055 Z-.0125 I-.2483

X-4.2564 Y.174 Z0. I.2496 J-.0004

X-4.1064 Y.424 Z.0125 J.17

G1 X-4.2564

G0 Z.1

Z.25

M5

G0 G28 G91 Z0.

M30

%

Yea I've hand coded a program like that and broke it up every 90 degrees but dont see how mastercam can do it without actually drawing out the path yourself.

Link to comment
Share on other sites
Colin Gilchrist Proficient

Colin Gilchrist

Posted
Posted

Yea I've hand coded a program like that and broke it up every 90 degrees but dont see how mastercam can do it without actually drawing out the path yourself.

 

As long as you've got Helix support enabled, "allow 360 degree arcs" turned on, and "Don't break arcs", Mastercam will output the Helix path, comprised of multiple 180 degree helix moves...

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

×
 Share
Go to topic listing

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...