[Robert M]

How to change the offset of a selected tool ?
From what I can understand at this point, the “Dia offset number” &/ or the “length offset numbers” are pre-set “somewhere” and each # as its own……offset value !?

How may I find these offset values attributes….and if needed ( this is the purpose of my present question and need ) change those values / offsets ??

Ref = Find all this in the tool manager, Dble click on a selected tool ( any ), then select “Parameters” tab

Thanks in advance for any help ....

[cadcam]

you can change them on the fly or are you asking to preset tools?
Maybe you are using a control that cannot have the tool # and the Dia and H the same as the tool so you need like Dia offset of 31 and H of 31 put the tool is T1

[Robert M]

Cadcan, thks for your reply.....but !!!! Hold on here....
allow me to be a little sarcastic
Are you describing this in....english ??
Or may be I should read this backward ....

Seriously...and don't take this any side other then....cheep sarcastic from me !
Honestly, I have not a clue what your suggesting...aside the "on the fly or preset" part.....shame for me !!
May you guide me more...."tutorially" .....needless to say, I've never done this

[cadcam]

Ok I will do that for you a little later off to dinner but I will get a video that will give you more in site to what I am saying.

(Seriously...and don't take this any side other then....cheep sarcastic from me !) All good LOL

[Robert M]

Great....
tks & enjoy a nice Sunday diner

[Robert M]

Cadcam.....no one else came forward !!?
Not to be....pushy.....BUT !
Any chance you may continue her ??

Appreciate !! Robert

[Superman]

you can change them on the fly or are you asking to preset tools?
Maybe you are using a control that cannot have the tool # and the Dia and H the same as the tool so you need like Dia offset of 31 and H of 31 put the tool is T1

you may not be describing your area of problems, for the correct answer, we would need to know what control, what the problem is, what solution you would like to achieve.

"on the fly" = means that you change the D & H offset numbers on the parameter page of each operation, as you create each toolpath
- some controls only have 1 set of offsets, ie geometry/wear ( not a D & a H page, to enable the use of offset numbers the same as the tool number )

now if you want to have Mastercam place the numbers automatically, permanent alterations are done thru the "control definition" page, which is 1st accessed by opening the "machine definition" ( accessing only the "CONTROL" file only does changes for the current part )

after opening the control file, tool change settings are in the "Tools" tab
- for an older Fanuc control, I use "Add to tool number" checked ON___Length(H) = 0____Diameter(D) = 30
( so T1 would give a H1 & a D31 ), or, by changing the T1 to T10 in the tool definition, H changes to 10 & D changes to 40 )
so I know that tool length would go into the same # as the tool number

"on the fly" in NOT the best method, forget to change just 1 op, could end in disaster ( CRASH )

- best to set all the tool parameter when you "create new tool" or when you load them from a tool file using the tool manager ( using the tool manager, think of it like that the lower area is your tooling cupboard, & the upper area is your tool carousel on the machine )

- any tool definition changes are then carried thru into all the toolpath operations
( any feed / speed alterations require a certain box to be unchecked in the config file )

[Robert M]

“you may not be describing your area of problems ”
I couldn't agree more !!

But to my defense….and many others requesting help…..a “good” question is as good as the basic info and / or knowledge you may have about….. it !
A paradox !!
So here goes / trying another way to expose it !

Trying to modify a T-slot cutter offset .
Logically, ( from what I understand at this point out of mastercam) mastercam uses the OD of the selected tool to follow the chain selected in the toolpath!
So fare….so good !
But….for my specific usage, I would like to have the discrepancy / the flexibility to change this “offset” of this selected tool in a manner so I can offset it from its center axis to follow this toolpath chain vs the “normal” way,.....it follows the outside cutting diam !
Make a long story….hopping this make sense !?

“checked ON___Length(H) = 0____Diameter(D) = 30
( so T1 would give a H1 & a D31 ), or, by changing the T1 to T10 in the tool definition, H changes to 10 & D changes to 40 ) “
Is this based on a “table” ??
Sort of a known value….of witch I can’t find ??
don'T quite understand ??
Where can I see / find the table values of these .....say “ T1 to T10”..... and others ??


I’ve never face this nor have a clue how to “play” with tool offset !
I can see from your explanation “ the tool offset register” in the control definition !
Would I assume correctly by thinking this modification will affect….all tools ?!

How my I change the “offset” of only one tool, a tool I chose for a specific chain ( as explain above here ?) ?

Thanks SuperMan, Robert

[seijack]

Sounds like you are talking about Cutter Compensation (Left, Right, None)

[Robert M]

" Sounds like you are talking about Cutter Compensation" Not quite !
Close, but with more flex !
more than a simple question of "left, right or...no compensation"
More like, say Ie : ...0.03125" from center axe !?!

[Superman]

Trying to modify a T-slot cutter offset .
Logically, ( from what I understand at this point out of mastercam) mastercam uses the OD of the selected tool to follow the chain selected in the toolpath!
So fare….so good !
But….for my specific usage, I would like to have the discrepancy / the flexibility to change this “offset” of this selected tool in a manner so I can offset it from its center axis to follow this toolpath chain vs the “normal” way,.....it follows the outside cutting diam !
Make a long story….hopping this make sense !?

Now we start to see where you need guidance, it is a tool compensation query
- nothing to do with H & D offsets


- it may be best to understand the relationship between your selected geometry, what tool you want to use, & what toolpath you expect when you set the correct options, in other words, chain --> comp values --> toolpath

- it depends on what entities you select for your chain, whether they define edges of your part, or added later for "other" machining methods

- if you select geometry that form the edge of a wall, you would need the cutter to also run along that wall, we typically, would use cutter compensation. Most would use climb cut when contouring(left), ( when selecting chains, the arrows play a big part in how the tool can be controlled, large=direction of cut, small=left/right comp )

comp type is how/what numbers are needed in the control to get correct tool "offset" to the selected chains
- "WEAR" is where the toolpath is already offset to the chain, the control requires a zero offset if the tool diameter is the same as programmed, ( a +ive offset will make the path stay further away from the selected chain, where a -ive offset will move the path closer)
- "COMPUTER" is where the path is adjusted by tool diameter in Mastercam only, the toolpath cannot be adjusted by offset in the control
- "CONTROL" is where the path is the same as the chain, the control requires comp to be the cutter radius
- "OFF" is where toolpath is the chain, no comp is used

Now for the added kicker
- the toolpath for each of these methods can be "adjusted" in Mastercam by using the XY offset allowance, ie create a roughing path operation that leaves say 0.2mm on a wall, and a finishing path op set to zero,,,,, all with the same tool, no alteration to the D offset in the control.


- there are many methods to get the same toolpath
if I want a path down the centre of a slot, I can
- draw a contour that is the down the centre & select that as my chain, set comp type to OFF, XY offset=0 ( +ive number moves the path in the direction of the small arrow seen when accepting the chain, -ive moves it the other side )
- using an edge chain, comp type=WEAR, XY offset adjusted to put tool on the centre ( comment as above, D offset=0 in the control will make the tool do the same path as seen on the PC )

say I have a 16mm slot, tool is a 26mm tee-slot cutter, selected chain is on the top of the 16mm wide wall, then I would need XY offset=-5 to have the cutter travel down the centre of the 16 slot....NOTE, lead in/out must be extended to allow tool plunge/retract outside of the part, suggest you use longer tangent lines & not use arcs

PS- XY offset is on the cut parameter page of that operation, lower section, it may be labelled "Material left on walls", can be +ive or -ive
PPS - process described is by using 2D Contour strategy & by selecting wireframe entities, not a surfacing operation

[fizzissist]

Had a new guy, new to CNC milling and programming, didn't quite grasp the whole offset thing. I said "let's take an hour or so and do an exercise".
We did a program in Mastercam that did 3 of the same profiles (a simple square) at different locations on a random chunk of aluminum, each using the same random (.5dia in this case) endmill. ... for safety we used ridiculously big lead-ins/lead-outs.
1st profile used wear comp, 2nd was computer, 3rd was control.

Got out the notebook, drew the square, then ran each profile... changing the dia offset as appropriate and starting the wear, computer, or control profile at its respective point in the program. We logged in detail the initial measurements of the profile using first the dia of the actual cutter, or 0 to see what happened. Then, we made adjustments in .02 increments, both positive and negative to the dia, and logged in detail what happened.

It was REAL tedious.

It was also really valuable to understand what happened when you did what, and how the control responds to what you do. We now have a very detailed set of notes that the next guy who comes in that doesn't quite grasp what it's all about can sit down and read.
Or, when the new guy asks me, I can just get out the notes and show him quickly.

[Robert M]

SuperMan…..
You really “wear” this nickname !
This is all ….SUPER !

It is so well explained and elaborated…it help allot !
It took me a day to reply as I needed time to ….digest all these infos…and when on tried ( tested) some of those and even when on combining some !
It was ( is ) a great lesson and learning steps as some of your detail steps made me realize many things ( initial conception when drawing, trying to compensate a drawing “mistake”, tool wear compensation…..and on).
I’ve enjoyed greatly this exercise ( reading and trying example form what you and others have suggested) and all this has open my eyes ( just goes to say many time we’re “blinded” in a “paradigm” mode !! ) and lack / suffer of looking / thinking “outside” on the box !
Maybe driven by stress or say pressure to perform, pressure to be efficient as what is expected….around a CNC w/ a software such as mastercam….being an efficient POWERFULL one !

The real fundamental problem, humbly, is what is known as a “code 18”
Yep, that’s right !!....18 inches from the screen was the real trouble…..ME !
Followed some intensive in depth courses on Mastercam several yrs back, but for personal reasons, had to change work orientation and was out of using it for over 3yrs…….which explains why I lost many simple Mastercam …..Functions / philosophy of usages !
Understanding MasterCam….as many detailed sophisticated software, requires staying “on it” using it on a regular basis !
But as the old say….goes…..it’s like cycling…..you don’t loos it, but may forget how to be a “performer” as being out of….intensive training !

All & all….
I’m happy to be back in the seat ( using it on a daily basis) and knowing there’s some great people like you guys in this community ready to back up some ( like me in this example) to the rescue….

Thks a lot……
Later, Robert

[Superman]

The real fundamental problem, humbly, is what is known as a “code 18”

Don't take this the wrong way...but
--your code 18 is also known as the "I Dee 10 Tee" error
( use letters for the syllables )

Glad you were able to make sense on the explanation
- I find that a lot of angst from new users comes from not knowing where items are found, or if it can be done. Let alone how it can be done.
You may have one way to get a usable toolpath, I may have another.....neither methods are incorrect.

There is no wrong way to create a toolpath that makes a correct part....only better methods.

Food for thought
- is it better.... to create a toolpath in 5 minutes, that runs for 10 minutes...or to create the perfect path in 30 minutes that runs for 3 min. ??
The only answer is...depends on the quantity

[Robert M]

So....
" I find that a lot of angst from new users comes from not knowing where items are found, or if it can be done. Let alone how it can be done."
So true......but none to blame, in my opinion, since Mastercam has ALLOT of "great" possibilities, hens, making it so flexible, yet, complexe and difficult to remember all if your out of it for some time, or not using it allot on a regular basis !!

Food....thought out !!
Is is better to spend 15 min to get an order out.....or 33min ??
I tell you, how much the customer will pay, how much time you can / must spend on it....

Later, Robert