HAAS-VF3 Post

[amckmp]

Post processor Help request

I am writing some programs for a friend with a HAAS-VF3.

Can anyone help with a suitable post

regards

amckmp

[email protected]

[mold100]

The mphaas post that is on your install disc should work well for what you are looking for.

[cadcam]

What are the problems with the Hass post you have?

[Ozzi]

I have a perfect one for $200

[Toby]

Ozzi - $200????? what's up with that and the foul language?

[Guest CNC Apps Guy 1]

Usually Ozzi, you need to prove your worth in here before charging such an outrageous figure for such a simple post. IMNSHO that's $50-$75 TOPS especially since Dave's MPMASTER is 99% there already and it's FREE!.

 

Contribute your vast knowledge for a while instead of just using the group to possibly get some work or money out of it. It's called "you scratch my back, I'll scratch yours". Truth is I rarely ever ask for anything in here, true that's my choice, but it's a good idea to contribute. It makes the forum better.

 

JM2C

[Eric S.]

Also take a look at the mpmaster post. It works well for the VF3 that I run.

[ROB]

or even mpfan works good and a few tweaks in the post if needed.

[Jim Whipple]

quote:

---

or even mpfan works good and a few tweaks in the post if needed

---

I use a tweeked Mpfan post that works well for my Haas also

I've been thinking of playing with the Mpmaster post just to see if I can Really screw things up!!

 

Jim

[MACHINEMASTERG]

what would it take to get mpmaster to output in caned drill cycles ??? g83 with i,j,k insteed of q?? and in g73 q and k ?thanks in advance

 

[ 12-09-2002, 05:38 PM: Message edited by: MACHINEMASTERG ]

[Roger Peterson]

What kind of machine tool is this for? A fadal?

[MACHINEMASTERG]

quote:

---

What kind of machine tool is this for? A fadal?

 

---

no a haas we have a post that was tweeked to do this and ive tried to duplicate what was done to it in the mpmaster post but no luck or no skills for that matter !! i like the mpmaster but the drilling could be better g83 i,j,k g73 q,k etc...

[Roger Peterson]

code:

---

 fmt  Q  2   peck1       #First peck increment (positive)

fmt 2 peck2 #Second or last peck (positive)

fmt 2 peckclr #Safety distance

fmt 2 retr #Retract height

fmt Q 2 shftdrl #Fine bore tool shift

fmt Z 2 zdrl #Depth of drill point

fmt Z 2 tosz #Drilling top of stock

fmt N 4 n_tap_thds #Number of threads per inch (tpi) / Pitch (mm)

fmt F 2 pitch #Tap pitch (inches per thread)

fmt R 2 refht_a #Reference height

fmt R 2 refht_i #Reference height

---

This is the portion of the post that controls the prefix for drill predefined variables. To use different prefixes with the same variable you will need to use the newfs function. Talk to your reseller about making the changes or if you want to learn purchase a post guide cd.

 

good luck,

[mark l]

While we are on the subject of mphaas posts, I have one that I have modified to fit my needs to a tee, except I have it were it post out the program number with what I have the file saved as, but it always puts a zero, for example if I save the file as 1111 it post out the number as O01111, I need the O but not the 0. Any help would be apreciated.

 

P.S. I don't know that much about posts, what I do is just trial and error, heavy on the error.

[MACHINEMASTERG]

thanks roger I WANT TO LEARN il buy it and try it !!!

[Roger Peterson]

MACHINEMASTERG

 

No problem.

 

Mark, check your format assignment. The corresponding format statement probably looks like this:

 

code:

---

fs2 xx 5 0 6 0l

---

The l makes all of digits before the decimal place output, even if it is a zero.

 

good luck,

[mark l]

Roger, I'm not sure if I understand you, my problem is the program number, this is what I get

 

%

O01111

GO G90

 

this is what I want

 

%

O1111

GO G90

 

I save my files for example 1111.nc, 2222.nc and I have my post post the file name as the program number but it puts that zero in it.

thanks again

[Finecut]

When i first posted out a file with the Hass post, just as it came on the cd I had My Haas dealer running a test job . The dealer in proofing the pgm on a VF-3 (Brand New) saw a G49 come up. Had he not been watching, it would have crashed the machine ( in Rapid ) This move is in the post in the toolchange section. Its not needed, and can crash depending how you set your length offsets. I took it out with a "#" in front of the line.

Also if you use a rotary on the machine you might as well make 2 posts. One with the "A" callout and one without. The Haas does not like seeing a rotary callout if its not on the machine and pluged in. This will save you the edit time.

 

Just my 2 cents

 

Finecut

[TheePres]

What is a G49?? My operator crashed machined when I started new company, 1st program. Theyr'e untweaked post (MPFAN) output this statement at header and I didnt realize the damage it would cause.

[Finecut]

It's a cancel cutter tool length. (G49)

Its the same as putting a H0

Iam looking for the file now. I belive the problem was that code was in the wrong spot when it came up. The tool was just above the part

Second the tools I belive were set (TLO) to a table probe. I was not there when the job was being set up but I was told the z axis was going for the table in rapid !!!

Just put a "#" in front of the line in the toolchange preretract as here:

 

#pbld, n, sgabsinc, "G49", pfzout, e

 

When I find the file (6 megs worth)I see what it did.

 

Finecut

[TheePres]

Output "G0 G17 G80 G90 G49 G40 "

The G90 mode is what caused this crash, I tested as such:

%

G91G28Z0

G91G28X0Y0

G49

G0G80G90G17G40

%

This way its harmless.

[MACHINEMASTERG]

we have that same g49 in our startup and never saw this??? in fack at the end of the programe it outputs g49 z0 before m30 and nothing like heading for the table ever happens???/

[mikee]

Threpres is right. G90 was active

G28 also cancels TLO but its called in g91 mode so the quill went to machine home. From looking at the file the tool would not have crashed, it just that the machine was running at 350 ipm when the tool was done.

I guess high feed rates and then going into rapid take a little time to get used to. The part was only 4 in sq. but "z" was moving at a nice clip.

The clearance plane was only .25 above the part, and the part was being roughed in 3d.

Ok so Iam the dummy, but I like to g91 g28 zo not g49. Safty I guess.

 

MIkee

[mark l]

I have had the same thing happen, I believe if you are actually calling up a tool length offset(H1) it will not do this, I think but it was such a close call when it happened I didn't want to take the chance on trying my thery.

[Fred from Université de Sherbrooke]

Mark l,

Don't know if somebody answered your first question but for your prog. number, you have to found to witch fs your progno is assigned

ei:

code:

---

fmt O 4 progno #Program number

---

and remove the l from the fs2 4

quote:

---

fs2 4 5 0 6 0l

---

l is to force the leading zero...