Z formula

readme · Jan 22, 2021

Who can help me with the formula.
I know how to calculate Z without tool nose radius. You see my formula.

Radius Compensation formula: tool radius - (tool radius x tan (angle / 2) ) = Z axis comp.

I don't get exactly the same result like Mastercam.

Mastercam code:
Z-4.685
Z-5.766

You know how to calc?

wmpy · Jan 22, 2021

What are you getting? I got 4.742 and 5.823 for the Z values. This is assuming all dimensions are in metric and you are cutting the external profile with a tool like a VNMG331. I don't know why Mastercam gives different numbers. Are you sure that the angle is exactly 45 degrees?

angelw · Jan 23, 2021

readme said:
Who can help me with the formula.
I know how to calculate Z without tool nose radius. You see my formula.

Radius Compensation formula: tool radius - (tool radius x tan (angle / 2) ) = Z axis comp.

I don't get exactly the same result like Mastercam.

Mastercam code:
Z-4.685
Z-5.766

You know how to calc?

Hello readme,
The formula is correct and will give you the TNRC Offset in Z. That then is applied to the actual part coordinate (No TNRC value). Accordingly, the values you have listed as Mastercam Code is only significant for anyone giving you help, if you also supply the actual part coordinate that relates to the values you've posted.

What are the following values supposed to be for?

Mastercam code:
Z-4.685
Z-5.766

A competent Finger Cam programmer would know off the top of their head, the X and Z TNRC for the common TNR for 30, 45 and 60deg angles. For the more obscure angles the above algorithm for Z is used and another for X.

Rounded to three decimal places, the above algorithm will present a value of 0.469mm for a 0.8 TNR and 45deg angle feature. If a 5mm x 45deg chamfer, starting at X25.0 Z0.0, is being cut, the following code for no TNR would apply. If you were going to commence the operation with the chamfer, you should start the chamfer from fresh air, say a 0.5mm standoff in Z.

G00 X24.0 Z10.0
G01 Z0.5 F1.0
G01 X35.0 Z-5.0 F0.25
Z-_ _
etc.

With TNR Comp for a 0.8 TNR

G00 X23.062 Z10.0 (X Comp = 0.938)
G01 Z0.5 F1.0
G01 X35.0 Z-5.469 F0.25 (Z Comp = 0.469)
Z-_ _
etc.

Regards,

Bill

Booze Daily · Jan 23, 2021

That brings back memories.
When I started on CNC lathes I finger cammed everything.
I had a cheat sheet of X and Z TNR comps for every angle.

EmGo · Jan 23, 2021

Booze Daily said:
That brings back memories.
When I started on CNC lathes I finger cammed everything.
I had a cheat sheet of X and Z TNR comps for every angle.

Why didn't you just program from the center of the tool nose radius and ditch the stupid tnr comp ?

Booze Daily · Jan 23, 2021

Not sure how that would eliminate the need to comp for tip radius?

readme · Jan 24, 2021

Diameter 16.662 have thread.

I can't believe mastercam give the wrong answer :scratchchin:

Nose 0.4

Mastercam code:
Z-4.685
Z-5.766

VS

Z-4.353
Z-5.434

Big different

Are you sure that the angle is exactly 45 degrees? YES

angelw · Jan 24, 2021

readme said:
Diameter 16.662 have thread.

I can't believe mastercam give the wrong answer

Nose 0.4

Mastercam code:
Z-4.685
Z-5.766

VS

Z-4.353
Z-5.434

Big different

Are you sure that the angle is exactly 45 degrees? YES

Hello readme,
I'm really not following you. Where is it that the MasterCam Code is incorrect? The following Z coordinates are correct for the drawing you've Posted and for a 0.4TNR

With regards to the MasterCam Z Coordinates and yours following, where you're going wrong is that you're not taking into account that the 45deg angle is being machined with the Trailing Edge of the tool.
Mastercam code:
Z-4.685
Z-5.766

VS

Z-4.353
Z-5.434

With the following algorithm to calculate the tool nose radius comp for a 0.4TNR and a 45deg angle

Z axis comp = tool radius - (tool radius x tan (angle / 2))

by plugging in the values you get:

Z axis comp = 0.4 - (0.4 x tan (45/2))

Z axis comp = 0.234

Apply this to the Z coordinates of the part Z-4.119 and Z-5.2 you get

For Z-4.119
Z Offset Coordinate = Z-4.119 - 0.4 x 2 + 0.234
Z Offset Coordinate = -4.685 (MasterCam Correct)

For Z-5.2
Z Offset Coordinate = Z-5.2 - 0.4 x 2 + 0.234
Z Offset Coordinate = -5.766 (MasterCam Correct)

Regards,

Bill

readme · Jan 24, 2021

Thank you... now I understand.

EmGo · Jan 24, 2021

Booze Daily said:
Not sure how that would eliminate the need to comp for tip radius?

Sorry, I knocked this out and it turned out not as illustrative as I'd like. I got too clever with the weirdo angles so it doesn't illustrate common things, like a chamfered corner. Hope you get the idea tho .... you write the toolpath to the dotted yellow line. That's offset from your part surface by the tool nose radius. It's like you're rolling a ball along the part surface. You can see how it uses arcs to go around the corners, so there is never a burr, the tool never leaves the part surface. And no need for tnr

It's actually easier and more controllable, just my example is poor

Please tell me it makes sense anyhow, or I'll have to do another one ... (supposed to be a round insert, by the way. Yes I know you can't normally cut on both sides with a cnmg)

View attachment 311459

sinha · Jan 24, 2021

EmanuelGoldstein said:
Sorry, I knocked this out and it turned out not as illustrative as I'd like. I got too clever with the weirdo angles so it doesn't illustrate common things, like a chamfered corner. Hope you get the idea tho .... you write the toolpath to the dotted yellow line. That's offset from your part surface by the tool nose radius. It's like you're rolling a ball along the part surface. You can see how it uses arcs to go around the corners, so there is never a burr, the tool never leaves the part surface. And no need for tnr

It's actually easier and more controllable, just my example is poor Please tell me it makes sense anyhow, or I'll have to do another one ... (supposed to be a round insert, by the way. Yes I know you can't normally cut on both sides with a cnmg)

View attachment 311459

For avoiding manual calculations, draw the line-sketch in AutoCAD, convert the lines/arcs into PLINE and thereafter use the OFFSET command, offset distance being equal to the tool radius. Finally, EXPLODE the offset curve (which is a PLINE) and extract information about the offset lines/arcs.

wmpy · Jan 24, 2021

wmpy said:
What are you getting? I got 4.742 and 5.823 for the Z values. This is assuming all dimensions are in metric and you are cutting the external profile with a tool like a VNMG331. I don't know why Mastercam gives different numbers. Are you sure that the angle is exactly 45 degrees?

Ignore these numbers that I gave. My calculator was set to radians instead of degrees. I agree with the Mastercam results.

angelw · Jan 24, 2021

wmpy said:
Ignore these numbers that I gave. My calculator was set to radians instead of degrees. I agree with the Mastercam results.

wmpy said:
What are you getting? I got 4.742 and 5.823 for the Z values. This is assuming all dimensions are in metric and you are cutting the external profile with a tool like a VNMG331. I don't know why Mastercam gives different numbers. Are you sure that the angle is exactly 45 degrees?

Hello wmpy,
Unless there is a drawing or Z coordinates given that I can't see in readme's first Post, I couldn't understand how you came up with any numbers whatsoever. All I could and can still see is the MasterCam coordinates.

Regards,

Bill

EmGo · Jan 24, 2021

sinha said:
For avoiding manual calculations, draw the line-sketch in AutoCAD, convert the lines/arcs into PLINE and thereafter use the OFFSET command, offset distance being equal to the tool radius. Finally, EXPLODE the offset curve (which is a PLINE) and extract information about the offset lines/arcs.

You can do that manually in DOS Bobcad really fast. I think it's even faster than acad, because the interface is quicker. Sometimes the Windows interface is a pain in the patootie.

Ox · Jan 27, 2021

Hope this visual aid helps:

Formula Z

1996%20SKI-DOO%20FORMULA%20Z%20583%20-%201.jpg

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

Think Snow Eh!
Ox

readme · Feb 6, 2021

I know how to calculate the first point (X48.766) but second don't know.This X52.266

How to calculate X52.266

Anyone know?

Ox · Feb 6, 2021

I don't understand the Q?

What is not known?

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

Think Snow Eh!
Ox

DouglasJRizzo · Feb 6, 2021

Unless it's a 1976 CNC, why not just program to part dims and use G42/G41 TNR?

readme · Feb 6, 2021

G41/G42 is milling - Radius Compensation.

Here can't use G41/G42

angelw · Feb 7, 2021

readme said:
G41/G42 is milling - Radius Compensation.

Here can't use G41/G42

Hello readme,
Of course you can use G41/G42.

However, following is the math.

X=(52.3+(Tan 43.747 x TNR) x 2) - TNR x 2

Regards,

Bill

Z formula

Plastic

Hot Rolled

Diamond

Titanium

Diamond

Titanium

Plastic

Diamond

Plastic

Diamond

Titanium

Hot Rolled

Diamond

Diamond

Diamond

Plastic

Diamond

Titanium

Plastic

Diamond

Similar threads