How can I lock these fields in Mastercam?

[Rocky16]

How can I lock these fields in Mastercam? I know it can be lock but I dont know how to do.

Thank for helping.

[Teh Bear without Brains kinda idiot]

iN CONTROL DEFINITIONS IN TOOL SECTION SELECT ADD TO TOOL

length zero diameter zero

 

HTH

[Rocky16]

iN CONTROL DEFINITIONS IN TOOL SECTION SELECT ADD TO TOOL

length zero diameter zero

 

HTH

Thank for your reply. But I want tool number and head and dia and len. offset can not edit in the yellow box.

How can I turn it to gray box and it can not edit. 

[Teh Bear without Brains kinda idiot]

Thank for your reply. But I want tool number and head and dia and len. offset can not edit in the yellow box.

How can I turn it to gray box and it can not edit. 

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

Use   the magic spell and wave your wand  .

 

Harry Potter cycle (G999)

Harry Potter in book #6
Will become CNC machinist
He will fight without wand
Only end mill in hond
And a caliper in left fist .

Harry Potter in book #7
Will find depths of hell ,heights of Heaven
Winds are blowing ,flowers growing
Magic sky strangly glowing,
And tool #13 offset value is 7

Harry Potter in book #8
Starts new spells to create
Magic spell for infinity ,
Total loss of virginity ,
Magic grip for a vacuum plate !

Harry Potter in book #bummer
Is outstanding moldmaker- programmer !
Life is cool,
Boss is nice
When you gripping in hands a sledgehammer !

Best regards
 

[CJep]

Thank for your reply. But I want tool number and head and dia and len. offset can not edit in the yellow box.

How can I turn it to gray box and it can not edit.

Short answer: there is no user setting that would allow you to do that.

[Colin Gilchrist]

You can lock Feed Rate, and Spindle Speed, but those are the only values you can lock on that page...

[jeff]

Thank for your reply. But I want tool number and head and dia and len. offset can not edit in the yellow box.

How can I turn it to gray box and it can not edit. 

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

Use   the magic spell and wave your wand  .

 

Harry Potter cycle (G999)

 

Harry Potter in book #6

Will become CNC machinist

He will fight without wand

Only end mill in hond

And a caliper in left fist .

 

Harry Potter in book #7

Will find depths of hell ,heights of Heaven

Winds are blowing ,flowers growing

Magic sky strangly glowing,

And tool #13 offset value is 7

 

Harry Potter in book #8

Starts new spells to create

Magic spell for infinity ,

Total loss of virginity ,

Magic grip for a vacuum plate !

 

Harry Potter in book #bummer

Is outstanding moldmaker- programmer !

Life is cool,

Boss is nice

When you gripping in hands a sledgehammer !

Best regards

 

HAHA! Did you forget to take your meds again?

[Teh Bear without Brains kinda idiot]

HAHA! Did you forget to take your meds again?

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

Yep. May I borrow yours ?

[Colin Gilchrist]

Alex,

 

A beautiful poem, and a perfect response...

 

Hope you are well,

 

Colin

[Rocky16]

How can I lock these fields in Mastercam? I know it can be lock but I dont know how to do.Capture.JPG

Thank for helping.

HI, I am back. I can do this very easy. 

And when you change your tool number, your leng and dia offset will be automatic change too. You will never worry about  unintentional changing dia and leng offset in every command. So what do you think?

[tiredtoolmaker]

That's great...so how did you accomplish this?

[Guest]

HI, I am back. I can do this very easy. 

And when you change your tool number, your leng and dia offset will be automatic change too. You will never worry about  unintentional changing dia and leng offset in every command. So what do you think?

I think I don't ever have this issue that requires your fix.

 

I don't mean that as a smarta$$ comment but to me, this is a solution in search of a problem.

 

Set your stuff up right, use good habits and you will never have the issue

[tiredtoolmaker]

Pardon me but I am simple minded and can see where Rocky's idea is useful. I have one machine to program, a Haas with a 20 tool carousel. With all the hundreds of tool #'s in the libraries, I always have to change the tool and length offset #'s. I always use the same # for each value. Am I wrong or don't have my stuff set up right? Again, I'm not programming a shop full of machines...just one.

[Guest MTB Technical Services]

Pardon me but I am simple minded and can see where Rocky's idea is useful. I have one machine to program, a Haas with a 20 tool carousel. With all the hundreds of tool #'s in the libraries, I always have to change the tool and length offset #'s. I always use the same # for each value. Am I wrong or don't have my stuff set up right? Again, I'm not programming a shop full of machines...just one.

 

 

You're doing it it wrong.

 

You create a library for your machine and it's done.

Very easy.

[tiredtoolmaker]

Ok I wrong but my 1/2" ball that's tool #5 today might be tool #7 tomorrow. I can't always use the same tool in the same slot. So once again, I'm changing tool #'s. Am I a total idiot for thinking this way?

[Guest MTB Technical Services]

Ok I wrong but my 1/2" ball that's tool #5 today might be tool #7 tomorrow. I can't always use the same tool in the same slot. So once again, I'm changing tool #'s. Am I a total idiot for thinking this way?

 

 

Yes.

 

You can simplify this process.

 

1) Create a library for your machine and set the initial tool numbers and offsets.

 

2)  Learn to use the Option in your machine setup in the Ops Manager that will sequentially number your tools for you as you add them to the current file.

 

3) Learn to use the tool renumbering available via right-click from the Ops Managers.

    This will allow you to renumber the entire file by the current order of operations.

 

 

All of this is basic training material your dealer should have covered.

If you skip training, this is the kind of thing you miss.

[Colin Gilchrist]

Ok I wrong but my 1/2" ball that's tool #5 today might be tool #7 tomorrow. I can't always use the same tool in the same slot. So once again, I'm changing tool #'s. Am I a total idiot for thinking this way?

 

Ouch, sorry if Tim came across as a little harsh with his response. In his defense, Tim knows quite a bit about running a machine and Mastercam in the most efficient way possible.

 

And there are of course, many different ways of setting up and running a machine, even a Haas. Which way is right? My answer is: the one you are most comfortable with, and the one that provides you with the most value is the one that is "right". It might be "right" for you, but would drive me or someone else crazy. So what. Do what works for you, and when you desire to look for a more efficient method, well this is just one of the many places on the internet that you can go for help and opinions.

 

For you, I'm guessing that the work you are doing on a daily basis is constantly changing, and the biggest limiting factor is the number of slots in your tool carousel. Even though you've got a lot of tools and holders, that may not get broken down. These tools might stay setup for a while, and just get loaded into the machine when necessary, even though the tool might now be in a different pot, and use a different tool number.

 

Does that sound like your working environment?

 

Even though I agree with Tim that his method makes it very easy to reuse tool definitions in the Tool Library, the issue it does create is the need to physically measure the Tool Length Offset and Tool Diameter Offset whenever you setup a new job. If you've got the Renishaw Tool Probe, this becomes a lot less of an issue, but you still have to take the time to measure the tools.

 

Depending on the Haas control you've got, some controls will allow up to 200 (or even 999) tool numbers, and TLO/CRC comp values. If this is the case, then it opens up new possibilities, as you could then manage the offset values independently of the tool numbers.

 

It still makes sense for you to setup and use a Master Tool Library. That is something that Tim and I can both agree on. When you define a tool, you should always add it to your Master library, that way you never have to redefine a tool you've already made in the past.

 

Let's say for example that you've got 200 offsets available on the machine, but still only have 20 tools available in your tool changer. I would recommend taking the most common tools you use, and setting these to be maybe the first 100 tools in the library (or 40, or 60, or whatever. It takes time and energy to setup a library). Take maybe tools 1-30, and make those common "Aluminum" tools. Then 31-60, and make these Steel. And then use 61-80 for Stainless. In these cases, the important thing is to set the Tool Number, TLO number, and CRC number. In the Control Definition, you can set Mastercam to read the TLO and CRC values from the Tool Definition. That way you could pull in Tool #56 for example, with H56 and D56. If you have "Number tools sequentially" turned on in the Tool Settings, you'd get T1, but still have the H and D value be #56. That way it would pull offset values that remain constant in the machine, even though the tool number might not be the same.

 

I will use a similar methodology for dealing with multiple TLO/CRC values for a single Tool Number. Say I want to use T11. But I want to be able to adjust the depth of a certain pocket, independently of the other pockets on the part. I might use T11, H11 to cut all the features except the pocket, then use T11 H111, to have the ability to "fine-tune" a feature at the machine.

 

I've got even further for other customers, by building some logic into the post processor to extract the actual TLO and CRC numeric data, and output it in the File Header using G10 offsets. This actually stores the H length offset number and D diameter offset value inside the Tool Definition itself. In this case, it would not matter what number values we put in the H and D offset, since we stored not only the TLO distance number (4.4521), but also the H value we wanted to populate with that offset number. That could be the Tool Number (so T=H, and T=D), but it could also be a different offset number altogether. (T11, H442, D335) The advantage to the system is that all of the data for a given tool can be stored and recalled by just grabbing that tool from the library. Unfortunately it also requires you to be diligent about recording the numeric data, and updating a given Tool Definition in your library.

 

So in your individual case, I could see you using a hybrid approach between what Tim suggested, and what I suggested. Have some tools setup as "static tools", where the offset data is stored on the machine, and some tools that are measured "on-the-fly". I've setup some machine controls to read an offset value of '999', for both the TLO and the CRC values, and if it sees a '999', it will automatically call the automatic tool measurement routine. This is also done with "Tool Groups", where there are say 6 of the same endmill, and they are called up based on a tool life parameter. Maybe I want to run a ball endmill for 50 minutes max, then change out the tool with a fresh one. This is all managed on the Machine Control side, but the offset is a "magic" number that invokes some macro logic on the control side.

 

If you have tools that always remain setup (same stickout, holder/collet, roughly the same gauge length), then set these tools up with some of the higher offset values. (Maybe 101-151?) So T101 might be your favorite 4" Steel facemill, T102 might be another 4" facemill, but for Aluminum. Set these tools and measure them (length and diameter), and store those values in those offset numbers on the machine. Even when you renumber your tools, you can keep the "static" offsets, and just have Mastercam call them up. So T5 might be H101. T7 might be H132. But you'll always have the correct offsets for that specific Tool, even though the numbers change. If you machine allows Tool numbers higher than the number of pockets, it becomes even easier. Just setup the specific tool ranges, and use those Tool numbers / Offset numbers, where everything still matches.

 

And a final piece of food for thought: I've also setup post processors to output a Machine Variable number for the D (CRC) and H (TLO) values. This is because the Tool Length value and the Cutter Radius Compensation value are always set to the "active tool number in the spindle". The machine is setup in such a way that the tool is automatically measured, and the H/D values stored to the tool number in question. You might use H#4020 and D#3020, and have only those numbers output for every H and D value in the program. Meanwhile, that is just set to the active tool number at the tool change...

[Rocky16]

Ok I wrong but my 1/2" ball that's tool #5 today might be tool #7 tomorrow. I can't always use the same tool in the same slot. So once again, I'm changing tool #'s. Am I a total idiot for thinking this way?

Hi,

Our shop floor use the same way like you, " 1/2" ball that's tool #5 today might be tool #7 tomorrowere. because we have many kind of parts with small quantity (1~5 pcs)  and our machines run 24/24. There is no tool list satisfy for all parts so we change tool list everyday. this part needs 5 tools but the other needs 20 tools, it is impossible to setup a fix tool list on CNC machine (30 tools on tool magazine). When I execute NC code I always set the same number for tool number, length offset and dia offset ( for instance: T3, H3, D3)

 

Moreover, sometimes in the night shift, operators can use our mastercam program for editing something like change the dia of tool ( maybe replace dia 3/4" by 1/2" cause there is no new 3/4" ) or view the simulation or tool path. in order to avoiding input wrong parameters because careless, I like to lock this filed.

 

I never change or edit or check parameters in this filed, If I have to change or edit tool, I always using tool manager.

 

In a mastercam program may be you have more than 100 tool path so it is not good if you have to check parameters in this field. I think if you do not use it when you make a NC program, you should lock it.

 

[Rocky16]

And I am waiting another poem from Ted Bear then I will show how to lock these fields. it take 25 seconds to do that.             

[crazy^millman]

Hi,

Our shop floor use the same way like you, " 1/2" ball that's tool #5 today might be tool #7 tomorrowere. because we have many kind of parts with small quantity (1~5 pcs)  and our machines run 24/24. There is no tool list satisfy for all parts so we change tool list everyday. this part needs 5 tools but the other needs 20 tools, it is impossible to setup a fix tool list on CNC machine (30 tools on tool magazine). When I execute NC code I always set the same number for tool number, length offset and dia offset ( for instance: T3, H3, D3)

 

Moreover, sometimes in the night shift, operators can use our mastercam program for editing something like change the dia of tool ( maybe replace dia 3/4" by 1/2" cause there is no new 3/4" ) or view the simulation or tool path. in order to avoiding input wrong parameters because careless, I like to lock this filed.

 

I never change or edit or check parameters in this filed, If I have to change or edit tool, I always using tool manager.

 

In a mastercam program may be you have more than 100 tool path so it is not good if you have to check parameters in this field. I think if you do not use it when you make a NC program, you should lock it.

 

Another way would be have the post ignore them. Post them the same as the tool number then you would never have to worry about them again.

[tiredtoolmaker]

Thanks for all the info guys. I did attend several classes and was bombarded with so much info it was impossible to digest. I scribbled notes which made little since when I returned to work. I depend on you guys for guidance since I have no one at work that knows anything about Mastercam.

[Rocky16]

Waiting for new poem

My way to do that: setting-->control definition manager.

[Colin Gilchrist]

Graying out the field does not "lock" a certain number or value into the data entry field. It just removes the option from the Tool Path interface itself. So if you want to remove access to setting those values, then removing the option from the Tool Path dialog by setting the option in the Control Definition will work.

 

So if all you wanted to do was remove the ability to set these fields, then yes, using the CD options to "gray out" the data entry fields is done just like you showed.

 

I think the thing that confused everyone (It confused me certainly), is the term "lock". In Mastercam, "locking" a field means to make the field "User Defined". Take "Cutting Feed Rate" for example. There is an option in the Mastercam Configuraiton that will allow you to "lock" the feedrate in the Operation. This will allow you to set a Feed Rate value of say "32.", and have that number not change, even when selecting a new tool.

 

Originally, I thought that is what you were asking for. The ability to set an offset value (Say "99"), and have that offset value be "locked" (user defined), and persist, even when changing to a new tool number.

 

Thanks for also posting up the solution to your problem, now that you've found it...

 

Best regards,

 

Colin