[MotorCityMinion]

Hello peeps, I'm new to this forum and hope this isn't posted elsewhere. Just getting started in a new job, day 2. Using a Haas VF series mill. Can I easily switch between absolute and incremental when I decide I want to tweak an offset, wether it be Tool length or WPC? I like using negative offsets for my WPC Z and haven't been able to find a solution yet. Same with Tool lengths, I may just want to change it by a few tenths and can't simply add or subtract .0003 to the offset. I can't stand touching off paper (Juvinile), as the Haas manuals imply is the usual way to set tools. (They dont like pre-setters?) They prefere that you leave WPC Z set to zero. LOL. I usually use a 1" block, then set my WPC to -1.00. I'll also use any block that is higher than my program Z zero to accomodate unconvention shapes such as Spherical rads, Angular work, and rounds, then measure from the top of the block down to Z zero, and input that number as a negative value in my WPC. This makes tweaking the entire set-up so much easier. Thanks for your replys

[HuFlungDung]

I'm not certain of your question but you can input values for your offsets in two ways:
input the value, and press "Write" which arithmetically adds the value of your input, to the existing value where the cursor is.
or,
input the value and press F1 to have the input value overwrite the current value.

[MotorCityMinion]

Perhaps this will help clarify my question. Inputting the data on the crt is a no brainer. What I'm trying to do is change the input mode to accept the data incrementally. Let's say I've set up a 17 tool job with several milling cutters in it. I run the 1st part, and decide I want to change H offsets 3, 7, and 11, by a value of -.0003 to do a better job of blending surfaces or compensating for tool pressure. On a Fanuc, Mitsubishi, or a Mazatrol controller, I can just go to the offset page (tool or wpc) and walla, there's a key that switches from ABS to INC. I do not have to touch the tool off again, then move it another .0003 to input the data. Nor do I have to add .0003 to the existing value and re-enter it. I just input -.0003 and press input. This is a fairly common routine. I've also used this technique to back-up or drive down a wpc Z value to suit my needs, or move a X or Y pick-up. I've haven't seen this capabilty on the Haas or mayby I'm just overlooking it. I'll try using the write feature and see if this does the trick. Thanks for your reply, MCM.

[cncdigger]

You can use the wear register in tool offset geometry and add or subtract whatever value to the tool lenght offset. The good thing is that your original lenght offset stays the same. This way, you always know by how much that tool has been feathered.

Al

[gar]

070226-1135 EST USA

MotorCity:

Hu has given you the answer that applies to all settings.

Cncdigger's suggestion is good because you can easily see the change you made.

Assuming you have a manual, if you do not it can be downloaded from the HAAS site. Look into the capabilities of G52. This is a very useful way to offset your coordinates from a base G5x. There are two modes for this HAAS and Fanuc. HAAS mode never automatically resets G52.

,

[MotorCityMinion]

Found it on page 113 of the PDF.
I tried the write key to add or subtract the values and it worked fine for both tool and work offsets. F1 replaces the value entered, while write adds it. The wear setting sounds interesting. G52? Meh, no need for that at this time. Day two on this controller and things are moving along fine. The guy thats training me has never used anything other than a piece of paper to touch off tools. His G54 Z's were also set to Zero. He's getting an eyefull at the moment. I also use a G43 Z1.00 Hxx, then on the first run, I'll stop the spindle at the initial Z and check the tool heigth with the same 1' block I touched off with. I had to change a setting, (64 I think?), to get the controller to use the actual Z position of the machine when setting tools and using a -1.0000 in my Z WPC.
There is a new Makino with a 20k RPM spindle and a heat shrink tooling system next to the Haas. Thats another controller I'll have to deal with in the near future and doesnt appear to be as simple to learn as the Haas. Hey, BTW, is the conversational quick code worth learning? Seems a bit weak at first glance. Thanks again for your help guys, MCM.

[cnc-king]

070226-1135 EST USA

MotorCity:

Hu has given you the answer that applies to all settings.

Cncdigger's suggestion is good because you can easily see the change you made.

Assuming you have a manual, if you do not it can be downloaded from the HAAS site. Look into the capabilities of G52. This is a very useful way to offset your coordinates from a base G5x. There are two modes for this HAAS and Fanuc. HAAS mode never automatically resets G52.

,

i would watch the G52, it could get you in a lot of trouble if you forget to reset the value.

[gar]

070302-2056 EST USA

cnc-king:

Why do you and so many others avoid using a very useful tool?

If you do not use tight control on how you use G52, then do not operate in HAAS mode. Instead use Fanuc mode where G52 is automatically reset to all zeroes under many conditions.

If you use a lathe then there is no HAAS mode.

There are many tasks where G52 is the most logical and efficient method to use.

If you use G54 with incremental offsets added to it thru a program, then you may be in worse trouble than using G52 in Fanuc mode where you would not modify G54 but simply change G52.

It is important to note that G52 applies to all G5xs simultaneously. What this means is: if there is a value in G52 other than zero and you change, for example, from G54 to G55, with G52 is unchaged, then whatever was in G52 before the change is there after the change, and thus G55 is modified by the same amount as was G54.

We always run our mills in HAAS mode and thus G52 is active, and we use G52. G52 is also always active in Fanuc mode, but if you always leave G52 with all zeroes, then G52 is effectively inhibited.

We set our tool lengths relative to a 1" gage block, usually from the left rear vise jaw. Then we use the G52 Z value to control our Z=0 plane. This is also very neat way to quickly raise the working area to do a dry run.

If step and repeats are not in our program, then usually the G52 X and Y values remain at zero.

.

[MotorCityMinion]

Hey peeps, thanks for all your input, This thread looks like it's starting to get off topic. Plese keep in mind that I'm talking about tweaking a multi part run in the initail set-up, or a 1 piece job. I do not endorse that operators change WPCs and G52s willy nilly through out a job run.

Gar to cnc-king: Why do you and so many others avoid using a very useful tool?

Motor replys as one of the "so many others": G52 intoduces another variable that has to be observed carefully and explained to everyone else. Just more room for errors, in my opinion. G54 through G59 are more than flexible enough and are common to every controller that I've used.

Gar: If you do not use tight control on how you use G52, then do not operate in HAAS mode. Instead use Fanuc mode where G52 is automatically reset to all zeroes under many conditions.

Motor replys: I don't willingly or knowingly operate in "Haas mode" or any other machine specific techniques. Keeping program codes and work piece coordinate setting methods as generic as possible and universally acceptable amongst many different machine controls, reduces set-up and programming time, errors, scrap, and keeps everybody on the same page. I suppose if a shop uses only Haas machines, this may be acceptable. I worked in a shop where the multi-pallet Mazak HMCs where beginning to out number all other machine controls. Our off-line programmer left the company and myself and 2 other shop floor personnel were programming in G code at the machine controls. We were sparsly using Mazatrol prior to this and management decided to make Mazatrol conversational the mandatory format. We're talking very large programs, machining engine blocks and heads complete. Most of the operators didn't have a clue as to how to read and edit Mazatrol. What a clusterf@#$ that turned out to be. I gave notice 3 days later, finished my last assignment, and haven't looked back.

Gar: If you use a lathe then there is no HAAS mode.

Motor replys: Not worried about the lathes or Haas mode.

Gar: There are many tasks where G52 is the most logical and efficient method to use.

If you use G54 with incremental offsets added to it thru a program, then you may be in worse trouble than using G52 in Fanuc mode where you would not modify G54 but simply change G52.

It is important to note that G52 applies to all G5xs simultaneously. What this means is: if there is a value in G52 other than zero and you change, for example, from G54 to G55, with G52 is unchaged, then whatever was in G52 before the change is there after the change, and thus G55 is modified by the same amount as was G54.

We always run our mills in HAAS mode and thus G52 is active, and we use G52. G52 is also always active in Fanuc mode, but if you always leave G52 with all zeroes, then G52 is effectively inhibited.

Motor replys: Sounds like trouble.

Gar: We set our tool lengths relative to a 1" gage block, usually from the left rear vise jaw. Then we use the G52 Z value to control our Z=0 plane. This is also very neat way to quickly raise the working area to do a dry run.

Motor replys: I agree with the 1" block or any other value that is higher than the actual work surface. I can't stand to see people touching off tools using paper or shims. I just back up the G54 wpc Z to use the same dry run technique.

Gar: If step and repeats are not in our program, then usually the G52 X and Y values remain at zero.

Motor replys: Lets hope so.

[gar]

070303-2012 EST USA

MotorCity:

Check setting 33 for the machine mode. Since you want to be sure G52 is zero at the start of your program you need to make sure that setting 33 is not HAAS.

One type of application where G52 is useful is the making of many identical parts from one piece of stock. For example 20 x 5 or 100 parts.

.

[MotorCityMinion]

I take it setting 33 is a default for haas? I'll check that soon. Perhaps the G52 is set to Zero and we've just been lucky for a long time. This was the end of my first week at the new job and I've found out that exploring machine options isn't a high priority here. Getting jobs running ASAP is. They load programs to the harddisk on the machine that uses 9 charaters with a file name that ends with A, B, or C, and so on to designate the order of operations for a given part. We can only download or upload 1 of those programs at a time because the machine only reads 8 characters at a time and will always overwrite the .ncc file. Thats silly. I'm working on changing that first. They also use a generic Post from mastercam that doesn't work and requires editing all the way through the program. Know where I can get a working post? I'll check the boards here 1st. Thanks for your time.

[gar]

070304-1053 EST USA

MotorCity:

I do not know if setting 33 is defaulted to HAAS, but it might be, and that is why I suggested that you look at its setting. If it is set to Fanuc, then G52 is zeroed at the start of CNC program execution.

We started with HAAS in 1993 and HAAS mode was the setting when we received that machine. On our other machines that range up thru 2000 I do not believe that we had to put them in HAAS mode, and they all are in HAAS mode.

If you are in HAAS mode and G52s are zero then you have just been lucky.

G92 works very much like G52. I have not but I need to investigate exactly what it does. The HAAS verbal description is inadequate. You will find G92 at the bottom of the G5x list on the offsets page where you would not normally see it. Check that these are zero. If G52 or G92 are not all zeros, then do not make changes until you record these values and the G5x values so you can reposition the G5xs as necessary.

On Mastercam check with the local rep for help on the post-processor. We use a generic Fanuc that we have editied to solve specific problems.

I am not sure about your question on filenames. We have our own Ethernet to RS232 System that we use for CNC communication.

However, some generalities on sending files to HAAS. I will view it from the RS232 perspective. If I put HAAS at the ALL position in the program list, then send a file to HAAS via RS232 the "O"-number at the beginning of the CNC program file is used by HAAS to store that program under that "O"-number in the program list. This has nothing to do with whatever file name was associated with the program in the Personal Computer. Basically the same happens from floppy.

The other option with floppy I can not describe now because I am not at the shop and only have the on-line manual available. The description in that manual is totally inadequate to consider your type of problem. The hard disk option will use a similar procedure to the floppy disk.

Basically HAAS does not care what the DOS file extension is. Therefore, you could create filenames like QWERTYUI.A, QWERTYUI.B, QWERTYUI.C, etc. However, this will be a inconvenience for most communication programs.

With our E232 System we work with long filenames and can send any number of files to HAAS without having to reset HAAS to receive for each different "O"-number. See our web site www.beta-a2.com for some discussion.

.