Help setting up 2 Vises, where i used to use one...

[jspangler]

Hi

Have a part that runs perfectly on 1 Vise, now need to set up 2 vises in the machine. First vise is G54, how do i set the program to duplicate the part at G55? Or how can I make it cut with each operation on both parts? Can I duplicate the part in MC8, and give the 2 parts seperate offsets? I'm trying to do this without having to actually measure the distance between the two vises and make a new drawing.

 

Thanks

 

John

[cadcam]

Yes sir you can an easy way is in the ops manger to copy each op after one another,

Now go into every other one and in the misc Integra on the first Parameter page.

Change the value to change the G54 to g55.

 

Now when you post it will use the same to and do G54 first and G55 right after in the code.

 

Hope this helps and makes sense.

[Keith Graydon]

Hmmm,

 

Lotsa ways to get it done. G54, G55, Copy and translate toolpaths...... but you'll still need to know the distance to the second offset. You could just plug in a value thats close. slap the second vise on the table to approximate that value and leave a lot of material to machine away to make up the difference.

Still easier to know the value.

 

my .02

hth

-KLG

 

-KLG

[jspangler]

Hi

Wow, thanks for the quick response. Now I can set the job up tonight.

 

That's what makes this forum so useful. After I read your reply, I was like " Duh", I should have been able to figure that out.

 

Hypothetically, what if the Z height of the second vise is different? Do I change that in the work offset in the control, or in MC?? Which is simpler, and which is safer?

 

Thanks again

 

John

[Roger Peterson]

Toolpath, next menu, translate: use toolplane positioning and if you have multiple operations and multiple tools pick by operation type, this will eliminate unnessesary tool changes, and in the lower right corner there is the work offset section set it so it increments to one starting with zero. on the translate page set it to one step in the Y and one step in the x and no distance between setups. This way you can set your work offsets at the machine and just indicate your stock or whatever your doing to pick up your G54 and G55.

 

hope this helps

 

I like to edit the z in the control

 

[ 09-03-2002, 02:45 PM: Message edited by: Roger ]

[cadcam]

You can do it in mastercam & machine by using a different "H" value for the g55 ops or you can use the machine and in the offset values change the "Z" value for g55 there.

 

If you are programming two parts different on the screen one for g54 And another for g55 then you do as roger said.

But if they are same part just program one like I said earlier and just copy and past in the ops manger and change the g54 to g55. I have one more thought using Xform let try some thing real fast.

[Keith Graydon]

John,

 

This is a solution for.....

 

quote:

---

Hypothetically, what if the Z height of the second vise is different? Do I change that in the work offset in the control, or in MC?? Which is simpler, and which is safer?

---

Give all the tools discrete Z offsets for the different vises.

 

T1 D1 (vise #1)

 

T1 D2 (vise #2)

 

saves editing.

 

HTH

-KLG

[JS]

What G55 value do you have to put in the control at the machine?

Thanks Joe

[cadcam]

JS most macines have a "Z" value that you can bascally raise or lower the table "Z" now take and eather + or - vale for the diffrence in the "z" from the fiest vise being G54.

[Keith Graydon]

JS,

 

The G55 value is from G54(vise #1) in X and Y. We're still discussing the Z value offsets

 

-KLG

[P_Scott]

John,

 

You could also Transform the toolpaths, Translate, by Tool plane, and check the box that says "Tool plane origin only". This will actually create a duplicate toolpath using the same values from the original part but at a new offset. If you "Copy source operations" and "Disable posting" you will be able to just post the Transform operation to get the proper code. Input the distance or find 2 points and tell it how many you want (copy 1 time). No matter what your actual distance is, your transformed toolpath will keep the same values as the original but with a G55 instead of a G54 after posting. HTH

 

I must've been slow in my reply because there were about 6 others that I didn't read from the original question. John, follow cadcam's advice for changing the "Z" value for the G55 offset at the control.

 

[ 09-03-2002, 03:33 PM: Message edited by: Peter Scott, SFA ]

[Keith Graydon]

Peter,

Youl still have to enter your g55 value in the offset register, No?

 

-KLG

[Tony]

JSpangler does your control accept Subprogram's (M98)?

 

[ 09-03-2002, 03:40 PM: Message edited by: Tony ]

[P_Scott]

Keith,

 

quote:

---

Youl still have to enter your g55 value in the offset register, No?

---

Yes, in the control you still have to set the proper offset register value. If the original part is at (X1,Y1,Z-1), "Transform-Translate-Tool plane origin only" will copy the values for the second part in the code (X1,Y1,Z-1). The only difference will be a new offset value (G55 instead of G54). Then the CNC machine operator only needs to touch off and input the offset (G54 and G55) values at the control to produce two duplicate parts. HTH

 

[ 09-03-2002, 04:18 PM: Message edited by: Peter Scott, SFA ]

[cadcam]

quote:

---

You could also Transform the toolpaths, Translate, by Tool plane, and check the box that says "Tool plane origin only". This will actually create a duplicate toolpath using the same values from the original part but at a new offset. If you "Copy source operations" and "Disable posting" you will be able to just post the Transform operation to get the proper code. Input the distance or find 2 points and tell it how many you want (copy 1 time). No matter what your actual distance is, your transformed toolpath will keep the same values as the original but with a G55 instead of a G54 after posting. HTH

---

Peter this what I was thinking about.

But I was looking for the place to change the offset to G55. thanks for answering that.

[Keith Graydon]

Thanks Peter,

 

I fully understand. (thanks to some great post of course!) I was trying to keep to JS's original question.

 

quote:

---

I'm trying to do this without having to actually measure the distance between the two vises and make a new drawing.

---

Anyway, Happy September. Kids are off to school today.

 

-KLG

[RandyN]

quote:

---

Anyway, Happy September. Kids are off to school today.

---

My kids have been in school for over 2 weeks now, different parts of the country.

[jspangler]

Hi

To answer questions in a few of the replies;

The control is a Haas (VF-2 2001), and to set the G55 ( or G54) I touch off the upper left of the vise and hit the tool offset button, scroll to work offset, and press the part zero button once for x and once for Y. That part I get. As for the Subprograms, the control does accept them, but i haven't used them except for a few of the exercises in the workbook when I first got the mill. Would this be better than transforming the toolpath? Also, is anyone familiar with the Haas quick code? i imagine i could use it for this setup and save alot of time by doing it at the control.

 

Thanks for all the responses. Just when i finally accept the fact that I am _not_ a machinist, you guys show me how to fake it for just a little bit longer....

 

Thanks

 

John

 

[Tony]

J

I use sub programming because it only has a few more lines of code.Tranforming is the entire original program times 2 or so etc.

My programs are sometimes twenty min loads!

 

Hit the Manual ,

see what format your control likes .

(From a G55,56,etc.Locating approach as opposed to an incremental way of positioning)

 

If you have four identical shapes in one block then I use Incremental.

 

Just another way to skin a cat

[lovemachine]

i have a haas and work with g54 and g55 in the work offset page you can also set Z on the offset page. Which is how i do it, it works well for me. If you sort by operation to reduce toolchanges you will go from g54 to g55) but will not g54 or g55 your Z (until your next z move). If there is a bigger diference in actual height than clerance above part WATCH OUT .

I read about that in a book

[MCFELIX]

i runing three diferent vises wiht 4 pcs in one vise

in the first vises is

 

G54 J1 1ST PCS

G54 J2 2ND PCS

G54 J3 3RD

G54 J4 4TH

 

G55 J1 TO G55 J4

G56 J1 TO G55 J4

[cadcam]

MCFELIX what is the Machine? thanks

[jspangler]

Hi

Help, I just set up the two vises, and vise two is .0264 taller than vise one. I set the work offset to compensate for it ( Z -.0264) according to the Haas VF-2 manual, and it seems to totally disregard this setting?

 

Help.

 

Thanks

 

John

[Scott Bond]

quote:

---

Help, I just set up the two vises, and vise two is .0264 taller than vise one. I set the work offset to compensate for it ( Z -.0264) according to the Haas VF-2 manual, and it seems to totally disregard this setting?

---

Hi John

I would like to ask you a few questions (just like if I was there)

Can you physicaly check the G54 X,Y,Z AGAIN? also make double sure to check that it is recorded in the code correctly.

Then physcaly check G55 and double check that it is recorded propper.

Also look at your gcode to make sure that you have G54's and G55's where you want them.

Don't spin out--You can do this!

 

If you are still stuck 818-772-4998

Then if you are still stuck I can make it in person sat. afternoon .

Scott

 

[ 09-11-2002, 09:44 PM: Message edited by: Scott Bond ]

[jspangler]

Hi

I checked everything. It's set up and running perfectly, but i can tell that it is cutting just a little too much ( i'm assuming .0264 too much) on vise 2. The haas operating manual says that to compensate for Z height, enter the value( which is .0264 higher than vise one), as a negative value, and it will raise the tool of the part by that much. This is in addition to the regular tool offset it is reading. It's set up right, but it's not working right. The other way to do it, by touching off the tools to vise # 2, and calling a different length offset / tool number will work, but i'm looking to make this a job that I can have one of the guys run, without a chance of screwing up a whole batch of parts.

 

Thanks

 

john