taping

[isse m]

hi fellows,does any one know good formela for taping blind hole 1/4-20 crs or any small tap for that matter.mastercam speed and feeds suck.

[J Coulston]

Do a search on MasterCam + suck, you will see that you are heading in the wrong direction.

[Lars Christensen]

isse m,

 

I would recommend you are using the feed and speed that you get from your tool supplier.

 

Lars

[Eeyore-nonhuman forum member]

Welcome to the board !

 

+1000 to John !

 

Not to offend you ,but first of all the question sux !

What is your material ,what are your job setup settings ,what are your tool settings ,what is a tooling (rigid taping or floating holder ) and do you know what speeds and feeds are good for your specific work at all ?

And what do you get after posting ?

 

Teh rigid

[mrainey]

quote:

---

first of all the question sux !

---

That was gonna be my answer, but you beat me to it!

[Dave anderson]

Im new to mastercam and have mostly figured it out on my own i have a smaller older cnc so when tapping i have to run in reverse so i pick left hand thread taps for my right hand tapping and always change the mastercam speed and feed to -100 rpm that way its easy to check your feed as mastercam i find adjust this for you i have tried both tension compression tap holders as well as just putting tap in collets rigid both have worked fine just make sure to verify spindle rpm i use this digital laser rpm thing with a piece of silver tape on the spindle works great for me . like i say im a novice but have never had a scrwed up hole or broken a tap. hope this somewhat helps you.

[Gary]

Damn these types of posts are getting old. If you don't think MC fills in the blanks for you on speed and feed good enough then put in your own! Krist it like saying a road sign says 45 for a speed limit on a corner but its icey as hell do you still gotta go 45? There are to many variables on things like this for mc to know exactly what we're doing. I just use them as guide lines because tools vary extreamily from one manufacture to another. I just punched it in mc and it came at 1070 rpm and haas programming instructor says to run it at 1400 rpm. This is for mild steel. I think its fast as hell but have done it and it worked.

[Rekd™]

quote:

---

If you don't think MC fills in the blanks for you on speed and feed good enough then put in your own! Krist it like saying a road sign says 45 for a speed limit on a corner but its icey as hell do you still gotta go 45?

---

x2

 

It can't do everything for you. There's always gonna be some intelligent and/or common sense input required by the user. This alone will determine your overall success or failure.

[Eeyore-nonhuman forum member]

~~~~~~~~~~~~~

It can't do everything for you. There's always gonna be some intelligent and/or common sense input required by the user. This alone will determine your overall success or failure.

~~~~~~~~~~~

+2T !

 

Also ,I found that Mc speeds and feeds tends to be too conventional for me ,and it makes a lot of sense ,you will never brake tool .

My speeds and feeds more aggressive ones .

I made tool libraries for most common materials and use them ,never calculate tool speeds and feeds from material .

 

[ 12-27-2004, 05:39 AM: Message edited by: Eeyore-nonhuman forum member ]

[Threept82]

The man is just asking a for help, as crude as it may be. I pretty much know or can find out tapping

speeds/feeds so I never check MCs. I just did. He’s right they do suck. I couldn’t find any percentage

adjustment area for tapping so if you didn’t know and went with MCs speed the tap, in his case would blow up.

If there is a adjustment area for tapping please let me know where and I will apologize.

[Threept82]

isse m

Blind hole in crs I would try S200 F10.0 staying

3 to 4 threads short if using a floating tapping head. If rigid tapping no need to stay short on depth and S600 F30.0 because it slows down as it

get closer to depth, you will probably never reach the full rpms anyway.

[Eeyore-nonhuman forum member]

~~~~~~~~~~~~~

couldn’t find any percentage

adjustment area for tapping

~~~~~~~~~~~~~~

This is specific to the tooling and controller !

Tweak your post to support it ,what the problem ?

Change your post text file and you`ll see

in misc .variables something as adjustment percentage and your postprocessor will be able to use it

~~~~~~~~~~~

Mastercam lets you set default values for up to ten miscellaneous integer values and up to ten miscellaneous real values from the NC Settings tab of the System Configuration dialog box (Main Menu, Screen, Configure, NC Settings). (Real values are floating-point or decimal numbers.) Any values that are set here are written to the NCI file at the beginning of each operation. Each value links to the appropriate value when you run the post processor. Miscellaneous values are available for Mill and Lathe toolpaths and wirepaths.

~~~~~~~~~~~~~~

Man ,if you don`t know something ,that does not means this thing not exists .

You can do anything with MC

Time for apology ?

[Threept82]

quote:

---

Man ,if you don’t know something ,that does not means this thing not exists .

Time for apology ?

---

Not quite yet.

isse m, was looking in Mc for S/F in tapping

changing a percentage or tweaking your post to support it helps him Not.. For in MC he should be able to tweak the percent value it the material

library so it shows up in his tool list.

[Eeyore-nonhuman forum member]

Be a man .

that`s your words

~~~~~~~~~~~~~~

If there is a adjustment area for tapping please let me know where and I will apologize.

~~~~~~~~~~~~~~~~~

I showed you where it is ,so what now .

Also ,who told you that all the floaters work the same way ?

And in rigid tapping your feed must be 100 percent

This is a proper way to do it ,if you don`t have rigid tapping ,insert adjustment percent in feed calculation inside your post and that`s all

~~~~~~~~~~~~~~

Not quite yet.

isse m, was looking in Mc for S/F in tapping

~~~~~~~~~~~~~

~~~~~~~~~~~~~~

hi fellows,does any one know good formela for taping blind hole 1/4-20 crs or any small tap for that matter.mastercam speed and feeds suck.

~~~~~~~~~~~~~~~

I can only guess for what he was looking

[Threept82]

I apologize.

You did tell me where to adjust.

 

But adjustments in that area is still pretty useless. If you need to change %'s on specific

material types then you would need to change txt file ea. time. Correct?

Sounds more feasible to be able to do it where you are and when you need it this

way its always there and F30.0 is 100% @ rpm of 600.

[Eeyore-nonhuman forum member]

No ,that`s very simple and easy and works like a charm . .

I will explain later :busy :

Someone ,explain to 3.82 how to use misc.variables .

PLz !

 

I accept your apology

Peace .

[Tim Johnson]

The idea of the misc. variables in this case is that you can change the percentage of MC's speeds on every operation needed. IMHO the best way to setup the "correct" speeds/feeds on a consistant basis is to create in the tool manager the tools you need for each material. After the tools are created and the speeds are proven you only need to click on the specific tool needed and save the effort needed to recreate the speeds every time you have to use a tool again.

[Eeyore-nonhuman forum member]

FIND THIS SECTION IN YOUR POST TEXT FILE

*.TXT

~~~~~~~~~

[misc reals]

1. "Misc. real [1]"

2. "Misc. real [2]"

3. "Misc. real [3]"

4. "Misc. real [4]"

5. "Misc. real [5]"

6. "Misc. real [6]"

7. "Misc. real [7]"

8. "Misc. real [8]"

9. "Misc. real [9]"

10. "Misc. real [10]"

~~~~~~~~~~~~~~

CHANGE IT TO

``````````````

[misc reals]

1. "Misc. real [1]"

2. "Misc. real [2]"

3. "Misc. real [3]"

4. "Misc. real [4]"

5. "Misc. real [5]"

6. "Misc. real [6]"

7. "Misc. real [7]"

8. "Misc. real [8]"

9. "Misc. real [9]"

10. " FEED ADJUSTMENT FOR TAPPING"

Ensure that appropriate misc variable switched on in *.pst file like this

~~~~~~~~~~~~

# --------------------------------------------------------------------------

# Enable/Disable Miscellaneous Real Variable switches

# --------------------------------------------------------------------------

1611. Enable miscellaneous real variable 1? y

1612. Enable miscellaneous real variable 2? y

1613. Enable miscellaneous real variable 3? y

1614. Enable miscellaneous real variable 4? y

1615. Enable miscellaneous real variable 5? y

1616. Enable miscellaneous real variable 6? y

1617. Enable miscellaneous real variable 7? y

1618. Enable miscellaneous real variable 8? y

1619. Enable miscellaneous real variable 9? y

1620. Enable miscellaneous real variable 10? y

 

~~~~~~~~~~~~~~~

in operation click on misc.values button you`ll see for your specific post

as 10`th misc.real

FEED ADJUSTMENT FOR TAPPING

enter the needed value like 0.85

 

Tweak post to use mi10 variable for tapping feed calculations

 

HTH

 

~~~~~~~~~~

the best way to setup the "correct" speeds/feeds on a consistant basis is to create in the tool manager the tools you need for each material. After the tools are created and the speeds are proven you only need to click on the specific tool needed and save the effort needed to recreate the speeds every time you have to use a tool again.

~~~~~~~~~~~~~~

Tim !

Some floating tape holders like tapmatic holders I work always need to be programmed with less feed than real to pull them out when entering tapeing hole and push in while returning ,as far as I know ,I think this is a thing ,3.82 wants

to achieve

 

Regards

[Threept82]

quote:

---

Tim !

Some floating tape holders like tapmatic holders I work always need to be programmed with less feed than real to pull them out when entering tapeing hole and push in while returning ,as far as I know ,I think this is a thing ,3.82 wants

to achieve

---

3.82 is not trying to achieve anything, I was answering a post question form someone else.

and with my tapmatic holders I have no problem

programming feedrate at 100%, sometimes I will

go up or down 10% on feedrate if hole accepts

no-go gage but thats rare.

[Tim Johnson]

quote:

---

Some floating tape holders like tapmatic holders I work always need to be programmed with less feed than real to pull them out when entering tapeing hole and push in while returning...

---

Eeyore,

You can change the thread pitch in the tool manager ex. a 32 pitch thread can be set at 37.647 threads (32 threads/.85)resulting in the same feedrate as Misc Real 10 would but you only need to create it once and rename the tool as "10-32 tap - tapmatic". This will also eliminate "forgetting to set the misc real 10" especially if you use both tapmatic and hard tapping.

[Eeyore-nonhuman forum member]

Tim !

+100 .

But 3.82 requested the feature And I show it to him

[jimspac]

What I do with tapping is to knock down rpm to level I am comfortable with. Once tapping cycle is selected, when you change rpm, the feedrate adjusts with it. I try to maintain whole figures on rpm and feedrate for rigid tapping.

[Tim Aydt Prototek Engineering]

I am suspicious of this guy. Could he be a spy?

 

[Eeyore-nonhuman forum member]

~~~~~~~~~~~~~~

I am suspicious of this guy. Could he be a spy?

~~~~~~~~~~~~~~

 

Teh ?

[Rekd™]

quote:

---

Teh ?

---

Negs..