Using a schedule program on a horizontal

[Shotout]

Just a quick question for you guys. The last shop I worked in I used a main program to call subs that where pallet specific, either one part or multiple stations per pallet. Real straight forward so easy a caveman can do it ya know. Well the shop I'm in now is currently awaiting a quote for a MA-500 so back to the horizontal I shall go. The initial basic setup is going to be two T type tombstones with 4 vises per tombstone. I'll be responsible for converting the programs that currently run on the verticals in vises, or fixtures mounted in vises over for the HMC. What I'm wanting to do is use a variable, one assigned to each vise number, that will be for the part counters. I want to end each program with a common variable+1 statement for part counting. Can I use a IF statement in the schedule program to check for the variable value and if it equals the count I input have it skip the main it is checking or does it need to be in the actual main program? I want to simplify things as much as possible for the setup guys, who are going to be blown away to start with by using actual tool lengths, center of rotation etc. Add to that multiple stations and differing part quanities on the same pallet and I can see some problems brewing. I figure a well commented general format program that is broke down into pallet one B0 Vise #1 H01 and so on will prevent to many problems, even more so since each vise will have a dedicated position and offset number for probing positions when required. New programs will be based of the center of rotation and a true position for each numbered vise as found with the probe or a bushing location that the fixture can be oriented from if the vises are off on a station or side. I've never programmed a horizontal for what is essentially a small production/job sized shop so any input or suggestions from those that do would be very much appreciated. I want to start off right so the training goes smoothly (consistent) rather than have to back track after finding out I didn't foresee something. TIA

I haven't read up on the formatting yet but basically
N100 IF [VC1 EQ 200] N200
N101 IF [VC1 LT 200] N102
N102 CALL OPROG
N200 IF [VC2 EQ....

[Superman]

A couple of questions, I'm reading between the lines.
-> is each vice is going to do a different component ?
-> is there any machining done at other than 0° and 180° ?
-> are the same parts to be done on the other pallet in the same position ?
-> if programming around the B-axis, this may limit your available options (ie. part programmed for RH vice cannot be done on the LH vice)


Bringing a program from a vertical to a horizontal then G11 P(angle) would need to be used, this in itself will be awkward for youself to set-up let alone have an operator try to follow it. IMO try using a program that is not transformed

Your answers may open an easier programming option
--a thought, you could use a plane or datum shift (G11 X[±value]) from the B-axis to a local point on the part

PS-- for additional functions for a horizontal-look at this thread

[Shotout]

Machining on 90 and 270 will be small parts being held in fixtures and programmed specifically for the pallet utilizing known true positions and the mastercam file will be offset at creation to match those positions. The dimension of those positions is too small for a regular vise and right now we only going to buy 8 Kurt vises. After mocking some dimensions the vises will be mounted so the fixed jaw will orient down towards the pallet. It should make them easier to load, clear the handles for closing them and provide chip clearing for the inside of the vise.

Each vise will do a different part, or in cases where a part is transferred op1 would be in a vise on pallet one and op2 on a vise on pallet two so each could have an individual variable to count the times it had been run. Of course I will also be machining the same part in multiple locations too, but for the most part we will be running several part numbers with differing order quantities on the same machine at the same time.

Converting them will be a requirement I'm afraid. We have a ton of repeat jobs on top of a load of 1st articles so this machine is a replacement for two small Fadals plus expansion. The only good news is that we just won a large part of a bid package we had out so a lot of the new part numbers will be coming to me as 1st articles. I'm kind of hoping to shunt as much of the conversion work over to the Okuma 4020s once this work starts to hit, it is a fast program conversion to change the program formats. Until then I am going to be responsible for keeping the spindle turning on a mix of repeat and 1st article jobs.

I had briefly looked at how to transform the angle of the part but as I am getting a jump ahead of everyone (waiting on trade in value and final price to cut the PO) I'm brainstorming right now and haven't actually read anything in detail. Once I get my ducks in a row I'll get into the details, and probably a few more options and ideas will open up based on this. AND I'll have User Task 2 again, YEAH! I've been missing it lately. I will be the primary person responsible for keeping the machine fed so my lead is giving me my head right now and we'll get together later to talk about it. Once I get things formulated a little more firmly I'll start running things by him for input and direction.

The thread you referenced. I have it printed out actually and it is in my MA-500 notebook. I've dug it back out and plan to read through it this weekend along with a lot of other samples I have for stuff I've used in the past plus things I've picked up from others that will be useful.

Thanks

[Superman]

Had a little think about how you may go about this

-> all programs must be able to run as a solo program
-> assign a # for each datum position for each vice ( use 1-10 for pallet#1 datums, 11-20 for pallet#2 )
-> a variable at the start of the program using the above # to define which pallet to be loaded, and done on which vice and also set the co-ordinate system
-> reset the variable to zero at the end of program
ie

N1 VC100=1 (  = 1st vice on pallet#1 )
       or VC100=12 ( = 2nd vice on pallet#2 ) ( this line deleted if running schedule program )
()
N2 T1   ( pre-stage 1st tool )
N3 IF [ VC100 EQ 0 ] ERR "VARIABLE NOT SET' ( a check that it has been set )
N4 IF [ VC100 GE 1 AND LE 10 ] M201 ( load pal#1 )
N5 IF [ VC100 GE 11 ] M202 ( load pal#2 )
N6 T1 M6 ( load 1st tool )
()
N7 G15 H=VC100
..
VC[VC100]=VC[VC100]+1 ( "broby" will correct me )
VC100=0
M30
%

schedule program ( it will need refining )
N1 PSELECT A.MIN, VC100=1
N2 PSELECT B.MIN, VC100=2
N3 PSELECT C.MIN, VC100=3
N4 PSELECT D.MIN, VC100=4
N5 PSELECT B.MIN, VC100=11
N6 PSELECT A.MIN, VC100=12
N7 PSELECT A.MIN, VC100=13
N8 PSELECT A.MIN, VC100=14
N9 GOTO N1
END

For the counting, I'm trying to get the # of the reference vice
so that counting is done by datum position

I'm also assuming you will get the custom macros going

this order save a lot of time at the start of the program
tool pre-select, then pallet change, then tool change ( in blue above)
while tool is pre-selecting, pallet change is also happening, and when complete, toolchange occurs

I hope you get the gist of where I'm heading
Steve

[Shotout]

I do thanks. It is what I was think towards. Like you said each vise will have it's own work offset # dedicated to it. All the converted programs that require edge finding will run in range and the offsets assigned to new programs will be dedicated but in a differing range. Once the tombstones are machined and vise positions established I can use the mnemonic expressions to rotate the program and offset the center of rotation to the the soft jaws or materials in the program origin so all tool lengths will remain valid as actual gage lengths. We do aircraft parts so there may be four programs using a #30 and 2 more using a #40 drill and all using a center drill so I want all tool lengths set by the reineshaw probe. I've got a nice little program that allows you do it manually and enters the values for length and diameter into the tool offset page for you. Kind of a nod towards protecting the probe. We'll probably end up with a presetter soon enough but until then the probe will be it. I appreciate the response and help.
scott

[broby]

In a schedule program, to set VC contents you must use the following format:

VSET VCxxx=yyy

where xxx is the variable number you want to set and yyy is the value you want to set.
Cheers
Brian.

[Shotout]

In a schedule program, to set VC contents you must use the following format:

VSET VCxxx=yyy

where xxx is the variable number you want to set and yyy is the value you want to set.
Cheers
Brian.

Thanks