Another no brainer

[Francis Farmer]

I'm still working my way through the exercises in the book, and Have a simple question. In the tool parameters box, on the far left hand side, third row down, is the DIA. OFFSET. In some examples it is 21, in others it is 25, What does this numerical value signify? I don't see a clear explanation regarding the Length offset which is the very next box below it (always a 1 in all the examples) in the manual either. Can anyone share some insight regarding this basic inquiry?

[Christian Raebild]

The 'dia. offset' and 'lenght offset' entries are the register numbers on the control, where the diameter offset and lengt offset values are stored. Whether they are output in the NC program depends on the post processor.

 

Unless you intend to actually cut the part, it does not matter what you enter in those fields. If you do intend to cut the part, then the values must be the correct register numbers, if they are used by the post processor and the control.

 

I hope this answers your question.

[Francis Farmer]

Christian,

 

If my processor is loaded correctly for the correct machine, can I just disregard these values? Will they be correct by default? Please excuse my ignorance.

 

-Francis

[Christian Raebild]

If your control uses the diameter and length offset values, then you may have to have the correct post processor loaded, and the correct configuration in the job setup. However, some post processors calculate the diameter and lenght offset registers automatically from the tool number, and some controls do not use diameter and length offset registers.

 

I cannot give a more accurate answer without seeing your post processor, but with your post processor on hand, I can give you an accurate answer in a matter of minutes.

 

Assuming your post processor works correctly for your control and machine, that is, and that the appropriate section of the post processor isn't protected.

[Francis Farmer]

I have the proper post processor loaded, as it is a Hurco Machine, and a Hurco p.p. I just couldn't understand why those values (the diameter offset and len. offset) changed by default for each different tool I taught into the system (with seemingly little bearing to the specified diameter of the tool), I wanted to have some sort of Idea of what there values correlated to. I am very new (I so far have written, posted and cut only the very simple contour and drill program in chapter 4), and in chapter 7 we are moving on into all of this business of loading tools into the program. As all of the tools are assigned an offset length and a diameter on the tool set-up page of my machines' controller, can I just leave the length and dia offset values on the tool parameter page in Mastercam at Zero, considering on the same page in the third column the tools' diameter is assigned.

[Christian Raebild]

Here is a simple test you can make:

 

Post process a program which uses cutter compensation in control, then change the diameter and length offset register numbers and post process it again (to a different file name).

 

If the post processed programs are identical, then you can disregard the offset register numbers on the tool setup page, if they are not identical, then you will have to enter the correct register number(s) for one or both offsets.

[Francis Farmer]

Thank you sir. I will do that before I go any further. Happy New Year.

 

-Francis

[Christian Raebild]

Happy New Year to you, too.

 

If your post processor and control use the diameter and length offset register numbers, then the control will use the diameter and/or length of a different tool if you do not enter the correct offset register numbers. Can you work out what then happens?

[Francis Farmer]

I read you loud and clear.

[Tony]

Francis

I have a Hurco VMX 30

Don't hesitate to ask me for anything

with Hurco/MC issues.

Tony

 

[ 12-27-2002, 11:51 PM: Message edited by: Tony ]

[Bud Jackson]

Am I correct when I say that the default value,

(ie: Tool #1 = H01..D offset = whatever, exmpl. 21/51 etc.) can only be set in the post?

I thought this could be changed/set in the Screen Config area but now can't find where.

 

I have mostly Yasnac controls and as rule begin Dia. offsets at 51=T1, 52=T2 etc.

 

Any help on how to get the Parameter pages to reflect this would be appreciated!

[d0gFartz]

Goto Main menu,screen,configure,select NC settings tab,toward the lower left click the Operation defaults button,select the defaults.df9 file (should be selected already) then click on save and it will open your ops manager that holds all your defaults,select the job setup button,in the tool offset register area make sure ADD has a dot in it then put 50 in under diameter,Ok out of that then Ok out of the ops manager then save your config file and then ok out of that...i would do a file new form the main menu and you should be adding 50 to the D`s now......Buddy dont forget about having administrative privlages though if your on that new computer so that the changes stay in effect

 

[ 12-28-2002, 07:41 AM: Message edited by: d0gFartz ]

[jeff]

Diameter offset is the number that you are going to use for cutter comp.(D VALUE)

Length offset is the number that you will use for the length of the tool at the machine.(H VALUE)

Example for Fanuc control:

G43H1Z1.

G01G41X5.125Y2.375D41F50.

[Christian Raebild]

quote:

---

I have mostly Yasnac controls and as rule begin Dia. offsets at 51=T1, 52=T2 etc.

---

Bud, if that 'rule' is what you use practically all the time, then coding the post processor to calculate the diameter and length offsets from the tool number might be an idea, though that means you will have to manually edit the NC code after post processing if you need a different offset register.

 

You can also use d0gFartz' suggestion, but you should be careful when changing the configuration in Mastercam, as you may accidntally make unintended changes. When making changes to the configuration, it is a good idea to select File -> New (resetting all settings to the current configuration) before opening the configuration dialog in Mastercam.

[Bud Jackson]

Thanks DOgFartz(Steve)..

Duh! Now I remember!!

As you and Christian both suggested, I saved it as a different file.."Mill9-50.CFG", and I must have administrative privlages , as it worked out fine even after re-boot.

Thanks Again

 

[ 12-29-2002, 10:55 PM: Message edited by: Bud Jackson ]

[heeler]

In the job setup screen, There is a box for offset Registers, You can check the box to add. Then if you want your length to be H1 (typ fanuc) leave 0 and put 50 in length for a D51 (typ fanuc).