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

[jspangler]

Hi

Just read a post from lovemachine I must have missed. This makes sense. If it is geting the G54 and 55's right, but not the Z's because that's what's happening here? Any workaround?? Seems like what i'm doing shouldn't be too uncommon, and it SHOULD work correctly. HAAS can't answer why this is happening, and I don't feel like dealing with Haas HQ today.

 

Thanks

 

John

[cadcam]

So john you changed the "z" value in the fixture offset for the other vise and it is not working?

I should of called you when I was my office I have a haas there.

[Jim Whipple]

If you tool offset on the lower vice....the Z offset in the G55 will be a pos value not a neg. as it (the G55) is taller or in the pos direction from the G54 if I understand your post correctly

Jim

[jspangler]

Hi

That's where I'm confused. In the Haas manual it says that to raise the tool 1" from the work offset, you would enter the value -1.00 in the Z offset of the part zero setting page. from lovemachines earlier post, he said that it doesn't look at the Z until a tool change. That doesn't make sense, but that's how it seems to be working. It seems like it should check the XY and Z position of your work offset before doing anything. I think for today, I am going to use different tool length numbering for vise 1 and 2, just to get the job outta here.

 

Any tips on getting this set up correctly would help.

 

Thanks

 

John

[TheePres]

Is your program outputting "Z" value at G55, it will not automatically shift Z just by going to G55 alone. Program should look as below:

 

(ex. drill holes)

G54G0G90X0Y0

G98G81Z-1.R.1

G55X0Y0Z-1. (z is required to compensate)

etc.

[Jim Whipple]

He is correct in that the program picks up the G43 after the work offset. When you set up two vices (at least this is how it works on My Haas at work ) I set tools to the G54 vice and use Zero in the G54 Z work offset register. Then when setting the G55 vice I put a positive Z number (to raise that offset) by the distance the vices are different

Works every time

Jim

[cadcam]

quote:

---

He is correct in that the program picks up the G43 after the work offset. When you set up two vices (at least this is how it works on My Haas at work ) I set tools to the G54 vice and use Zero in the G54 Z work offset register. Then when setting the G55 vice I put a positive Z number (to raise that offset) by the distance the vices are different

Works every time

---

Jim this is how I do it in my Haas to this what I was talking about in the offset page.

[Jim Whipple]

Jay:

I was just trying to point out that the shift was pos as opposed to neg when the g55 was higher than the g54

We're talking the same thing I think

Jim

[cadcam]

Jim yes we are.

[SLJ]

Guys and Gals

We use different vises and fixtures often. I set my wcs for each vise or fixture where the operator can get to it easily. Program each location from that wcs, then the operator sets all tools from the G54 location Z0. All he has to do is set G54 and G55 XY0 at their location, then put the difference in Z from G54 to G55 in G55 offset(including sign). If using a tool probe or seperate tool setting block o set tool length offset, you would just touch off the first vise to set G54 Z0 and then input the diff. in the vises in G55 Z. As was explained earlier, watch the clearance value if there is much diff in Z's.

[jspangler]

Hi

I got it to work. What i did was measure the tools using the taller of the two vises, and then enter the z value for the first vise (-.0264).

Before, I was touching off the shorter vise, and attempting to add the .0264 to the Z of the second vise. The control didn't like it , but everythings working like it is supposed to now.

 

THANKS for all the quick responses.

 

John

 

BTW, just having the second vise, on a 7 tool op, (with 9 changes), cut time from 28 Minutes EACH part to 40 minutes for 2!!!

Now if I could just fit One more vise in there....

[McRae]

Check out a double acting vice from Parlec of Chick. The name of the game is - Parts to the Spindle... The more parts you can fit on the table, the more you can amortize cycle time, tool change time, pallet change time, part change over - etc. Watch out though as scrap rates can soar if the process isn't stable (or if the operator changes the wrong offset.)

[BernieT]

quote:

---

Watch out though as scrap rates can soar if the process isn't stable (or if the operator changes the wrong offset.)

---

You will notice that ALL Machines run scrap at approx 3 to 5 times faster than normal rates!!

 

BerTau

[Jim Whipple]

quote:

---

You will notice that ALL Machines run scrap at approx 3 to 5 times faster than normal rates!!

---

Well Boss, I got good news and bad. The bad news is I scrapped 3 parts. The good news is I'm getting faster!

Jim

[cadcam]

quote:

---

Well Boss, I got good news and bad. The bad news is I scrapped 3 parts. The good news is I'm getting faster!

---

ROFLMAO

[Guest CNC Apps Guy 1]

Run scrap...... LOL!!!!!!

 

Well it could be worse. Our resident MORON on second shift, toasted a spindle in one of our Mori Seiki's the other day, so if I had to choose between running scrap and smoking a spindle, I'd take the scrap. $10,000 for the new spindle in case you were wondering, and yes he still has a job. According to my calculations, the guy has cost the company about $15,000 in the last month to two months.

[Hacsta]

Hello, new to the forum,and mastercam. I'm trying to transform translate toolpath but when I post(mpmaster.pst) it just outputs g54. what can i do to make it output multiple workoffsets for the translated ops

[Hacsta]

oops!! v9sp1

[McRae]

Use MPSUBREP

[P_Scott]

hacsta,

 

Welcome to the forum and I like the handle. When translating toolpath you have two methods to do it, either by Tool Plane or Coordinate. In the latter, you will only add the distance value you supply from the original part you are translating. With Tool Plane, you have the option of assigning different work offsets to your translated toolpath. If you use Tool Plane and want the same coordinate values for each part, just with a different work offset, select the "tool plane origin only" switch under the Translate type switch. HTH Also see previous posts in this topic.

[Hacsta]

thanks for the info guys, I will try these out and get back to you

[Hacsta]

the mpsubrep works great just what i was looking for! thanks for the help,