Can someone give me an example of the syntax for an "IF" statment ?

Heres what we would like to do. As of now they use two different programs for the same part, program one is for pallet 1 and program two is for pallet 2.

Would be nice to use one program and set a variable at the beginning to control what workshifts to use (yes, consistent fixtures would be nice :) ) .

Example.
P01 = pallet one
P21 = pallet two

N001 PL = 1
N002 IF PL = 1 THEN G54.1 P01 ELSE G54.1 P21

Then we would just edit line N001 when needed.

Is this possable, never did anything like this with a CNC program before, but seen some stuff which is close in a few threads around here.

Using a FANUC 16i control.


_

060726-1501 EST USA

iMisspell:

I do not know Fanuc details, and I am not where the HAAS manual is.

On HAAS I would use G5x (in your case G54) as the base zero reference. This might be a location near one corner of the pallets. Then I would use G52 to offset from the G54 to the work zero for your part. This hopefully will be clear in the following example.

If there is a machine variable that contains the the pallet number, assume for the following example it is #3028 (pallet number in receiver from HAAS manual on line -- I do not know what this is because we do not have a pallet changer machine), and that a 1 in this variable is pallet 1 and a 2 is pallet 2, then we can make your part zero relative to machine zero automatically set based on which pallet is in the machine. This is automatic as follows:


You can either manually load G54 before you run the program or G54 can be loaded at the start of the program. But this G54 value will remain unchanged from part to part and pallet to pallet. So will the two different G52 values remain constant, but the ones loaded into the G52 location are determined by which pallet is in the machine.

Within your program you will have

IF [ #3028 NE 1 ] GOTO 110

N100
G52 X5.1260 Y4.8796 (for pallet 1 work zero from G54)
GOTO 130

N110
IF [ #3028 NE 2 ] GOTO 120
G52 X5.1753 Y4.9903 (for pallet 2 work zero from G54)
GOTO 130

N120
(Pallet number error)
M00


N130
(Your common program is here)


.

Thanks for your example and explanation, gar.

Ive seen the GOTO and understand its use but think it would be a bit of a pain to implement for us.

In short, heres the my situation. I was just moved on a machine in a prodution shop which has been running programs and parts for a while now (2-3 years). Ive been re-doing some of the programs but do not want to make two programs for each part (a program for each pallets Work-Shift with the only change being a P0# to P2#).

Cutting a four sided casting they use a G54.1 and P# to set the origin for each side, pallet one would be P01=SideA, P02=SideB, P03=SideC, P04=SideD and P05 to control the bores (the old programer tryed to set up the programs so a compleat simpleton can run the machine and theres no real set-up to do, just plug in a few numbers and their done, i have to keep it like that, which is not my choice) for pallet two would be P21, P22, P23, P24, P25. I like the G52, but that would cause alot of confusion for the other guy running the machine, i cant make alot of "radical" changes.

Anyway...
Tool 1 is called up, does some work on Side-A which is P01, then the pallet indexs to Side-B and P02 is called up, all in the same operation. If we were using pallet 2 it would be SideA=P21 and SideB=P22.


Heres a clip of one op (i edited out all the cutting lines)...

(T2, 4" FACE MILL, FINISH 4 SIDES)
N008 G54.1 P01 (work-shift SIDE-A)
.... edited-out ...
N016 G53 Z0.
N017 M01
N018 G0 B90.
N019 G54.1 P02 (work-shift SIDE-B)
.... edited-out ...
N049 G53 Z0.
N050 M01
N051 G0 B180.
N052 G54.1 P03 (work-shift SIDE-C)
.... edited-out ...
N060 G53 Z0.
N061 M01
N062 G0 B270.
N063 G54.1 P04 (work-shift SIDE-D)
.... edited-out ...
N095 G53 Z0.
N094 M01
N095 M06
N096 M01


So for what your saying i would have to do somthing like this ???

Default the code for P01 (pallet one) and use the IF's to skip over them if we're gonna use pallet 2...

(T2, 4" FACE MILL, FINISH 4 SIDES)
IF [ #3028 NE 2 ] GOTO 100
N008 G54.1 P01 (work-shift SIDE-A)
GOTO 101
N100 G54.1 P21
N101 X0 Y0 Z0
.... edited-out ...
N016 G53 Z0.
N017 M01
N018 G0 B90.
IF [ #3028 NE 2 ] GOTO 200
N019 G54.1 P02 (work-shift SIDE-B)
GOTO 201
N200 G54.1 P22
N201 X0 Y0 Z0
.... edited-out ...
N049 G53 Z0.
N050 M01

ect...


I dabble with VB (Visual Basics) and some other simple PC programing langs and was hopping that there was an 'ELSE' command that whent with the IF statment's.

For the ease of editing i was hoping there was somthing along the lines of...

(T2, 4" FACE MILL, FINISH 4 SIDES)
IF [ #3028 NE 1 ] G54.1 P01 ELSE G54.1 P21
.... edited-out ...
N016 G53 Z0.
N017 M01
N018 G0 B90.
IF [ #3028 NE 1 ] G54.1 P02 ELSE G54.1 P22
.... edited-out ...
N049 G53 Z0.
N050 M01

ect...


Less to edit and i would not have to pay attention to line numbers, one less mistake which can be made :) .


------



Anyway...
When using the IF statment, NE is the equivalent for = (equals) ?


Thanks again for the example, ger.
- joe


__

Since you only have two conditions, why not just write two IF statements, on two lines?
In computereez, when an IF condition is false, no further processing takes place on that line.
An Else function may be too high order in command language for your cnc to interpret.

060727-0728 EST USA

iMisspell:

If I understand your original question --- you have two pallets and the parts machined on these pallets are identical, but each pallet clamps in the machine in a slightly different position than the other one. Therefore, you effectively need different values in G54 for pallet 1 than for pallet 2.when clamped in the machine.

Your second post introduces an unexpected factor, rotation. If you simply changed from one set of values in G54 for pallet 1 to a different set of G54 values for pallet 2, then would this cover all four rotational positions. My guess is not. That would mean that you actually required 4 different G54 sets for each part or a total of 8. This can be handled fairly easily, but I need to know if this is what is required, and do you have G52 that provides a modification to G54 without changing G54.

If you do not have G52, it is not a major problem, just a different route.

Do you have G65 which allows passing paramters to a subroutine?

.

Actually, you could just use IF statements to read G10s and use the same offset call for both pallets.....

IF [ #3028 EQ 1 ] GOTO 100(PALLET 1 OFFSETS)
IF [ #3028 EQ 2 ] GOTO 200(PALLET 2 OFFSETS)

N100
G10L2P1X??Y??Z??B??(G54 FOR PALLET 1)
GOTO300
N200
G10L2P1X??Y??Z??B??(G54 FOR PALLET 2)
GOTO300

N300(START PROGRAM)



Simple and easy and one program. G52 will work as well, but a lot of people today don't understand G52 and its relation since its not that common anymore in many places.

Can not use the else statement, so I just do it first then run my if:

N001 PL = 1
N002 IF PL = 1 THEN G54.1 P01 ELSE G54.1 P21

N001 PL = 1
G54.1 P21
N002 IF PL = 1 THEN G54.1 P01

My pallets are set at parameter #1000 and #1001 but I think that might vary by the machine manufacturer.

O7999
N010
#1=0.(SAFTEY CHECK)
IF[#1001EQ1]#1=1.(PALLET #1 ID)
IF[#1000EQ1]#1=21.(PALLET #2 ID)
IF[#1LE0.]THEN#3000=54(WHAT THE HELL W.O. ALARM)
N020
G54.1 P#1
N100
M99

In my main program I run;
M60(PALLET CHANGE)
G65P7999(SET WORK OFFSET)

Tom G

060727-1159 EST USA

iMisspell:

EQ is the logical function symbol for equals (a comparison function)
others are NE for not equal, LT less than, etc.

= is a symbol for inserting a value into a variable
#100 = 1.23 causes the number 1.23 to be put into variable #100 obviously destroying what was previously in #100.
#100 = #101 causes the content of variable #101 to be put into #100.
A more descriptive symbol might be
#100 <= 1.23 where <= means copy the evaluated value from the right side to the variable on the left side.


psychomill's suggestion is a simpler way. In HAAS it does not always work, and is dependent upon the function following the implied THEN.

What the G10 L2 P1 command does is to overwrite the contents of the variables that store the G54 offsets. Only the axes listed as parameters in the G10 command are overwritten.
In HAAS some of the addresses are
#5201-#5205 G52 X, Y ....
#5221-#5225 G54
#5241-#5245 G55
etc.

Assume that G54 is the current work offset, then in a HAAS mill in either HAAS or Fanuc mode the G52 values are added (added may mean subtracted) to the currently selected work offset (G54) to produce the actual work offset, but the value in the current work offset (G54) is not modified. For example:
#5201 is added to #5221 to generate the actual X work coordinate.

When the G52 values are all zeros the current work offset is the actual work offset.

Suppose you make G54 the work offset for the part zero for pallet 1 side 1. Then the values you would load into G52 would be the offsets from that one reference position to the corrected position for the other faces and pallets. In other words the contents of G52 would be the error in part positon relative to the position for pallet 1 side 1.

G52 is a very powerfull and useful tool in HAAS. In HAAS mode the values in G52 are retained even thru power down or program changes. In a HAAS machine in Fanuc mode G52 is zeroed on power on, program start, and some other conditions.

.

Since you only have two conditions, why not just write two IF statements, on two lines?For the ease of editing and being that my hands are tied on the extent of editing i can do, im gonna try what thogib posted.

PL = 1

G54.1 P21
IF [PL = 1] G54.1 P01


Your second post introduces an unexpected factor, rotation.

...Do you have G65 which allows passing paramters to a subroutine?Sorry, i should have mentioned the table rotation.

These programs are straight-up simple CAM programs, no subroutines of any sort (at least not that ive seen yet.) (i can post one if your bored and want to peek at it).


Actually, you could just use IF statements to read G10s and use the same offset call for both pallets.....

Simple and easy and one program. G52 will work as well, but a lot of people today don't understand G52 and its relation since its not that common anymore in many places. Im gonna try this some tiem when i get time, but i do not think my partner is gonna be too keen on this, his not real big on change :( Plus im not wrting the programs from scratch just editing them to fine tune them alittle, i just counted how many P0#'s (pallet rotations) in one program and it was 22, setting them all with G10's is alot-like-work for someone thats a bit lazy ;) But for learning im gonna give it a shot on an op or two.


thogib
Im new to Milling (and subroutines (but understand the concept from PC programing)), from the reading ive done, thats somthing which i would like to do, but i know the other guy running the machine would flip, then he would have to keep track of what program numbers not to delete from the control and having two O### printed out or in the same file... just wont work with him.



EQ is the logical function symbol for equals (a comparison function)
others are NE for not equal, LT less than, etc.

= is a symbol for inserting a value into a variable
#100 = 1.23 causes the number 1.23 to be put into variable #100 obviously destroying what was previously in #100.
#100 = #101 causes the content of variable #101 to be put into #100.
A more descriptive symbol might be
#100 <= 1.23 where <= means copy the evaluated value from the right side to the variable on the left side. Copy/Paste and print :) thanks.
Its nice to see they keep the syntax close to other programming langs, those attributes can be used with PC SQL-DataBase work.

gar, thanks alot for your explanations, im sure it will help others reading this thread as well for the help you've been to me.


Another question.
At the beging of the program im gonna define PL = 1
Will the PL varable hole the value of 1 after we hit the Rest button on the control ?
I would think it would loose its value once the machine is powered down but what about just hitting the re-set button ?

Thanks again to every one, been a big help, nice to see different paths that can be takin.


_

i just counted how many P0#'s (pallet rotations) in one program and it was 22, setting them all with G10's is alot-like-work for someone thats a bit lazy

Yes, but you only need to set the G10 once at the top of the program, not 22 times through out the program. If you're using say 6 ofsets, then you could write it like this:

IF[#3028EQ1]GOTO100(PALLET 1 OFFSETS)
IF[#3028EQ2]GOTO 200(PALLET 2 OFFSETS)

N100
G10L20P1X??Y??Z??B??(G54.1 P1 FOR PALLET 1)
G10L20P2X??Y??Z??B??(G54.1 P2 FOR PALLET 1)
G10L20P3X??Y??Z??B??(G54.1 P3 FOR PALLET 1)
G10L20P4X??Y??Z??B??(G54.1 P4 FOR PALLET 1)
G10L20P5X??Y??Z??B??(G54.1 P5 FOR PALLET 1)
G10L20P6X??Y??Z??B??(G54.1 P6 FOR PALLET 1)
GOTO300
N200
G10L20P1X??Y??Z??B??(G54.1 P1 FOR PALLET 2)
G10L20P2X??Y??Z??B??(G54.1 P2 FOR PALLET 2)
G10L20P3X??Y??Z??B??(G54.1 P3 FOR PALLET 2)
G10L20P4X??Y??Z??B??(G54.1 P4 FOR PALLET 2)
G10L20P5X??Y??Z??B??(G54.1 P5 FOR PALLET 2)
G10L20P6X??Y??Z??B??(G54.1 P6 FOR PALLET 2)
GOTO300

N300(START PROGRAM)
.
.
.


Then you use the same program, same offset calls to run both pallets. You won't need to do this:
Tool 1 is called up, does some work on Side-A which is P01, then the pallet indexs to Side-B and P02 is called up, all in the same operation. If we were using pallet 2 it would be SideA=P21 and SideB=P22.


Just use the one program and one set of offsets.

:cheers:

Bad new for me :(
Tried the IF statments and it kicked up an error, bad macro (or somthing, wrote it down but forgot the paper at work, i know the word 'macro' was in the error.) recived this same error when trying to set a varable, PL = 1. When keying in the ...
PL = 1
it would input...
P L =1
(space between P and L and removed space between = and 1), so i tried A=1 and kept getting the same error, didnt have time to play around.

psychomill
After re-reading what gar post, i now compleatly understand what you are saying and actuly think the day guy will like that, alot. Since we cant get the IF's working right now, maybe ill just write in both (pallet A and B) and then when we start the run we can just delete or skip/block what ever set we dont want to use.


_

060728-0632 EST USA

iMisspell:

More questions.

On your pallet is there one part, or is it a tombstone with many parts?

Assuming it is one part, then is it a raw blank, or has it had previous operations performed?

These questions relate to whether you need different work zeros for each rotary position of the pallet, or just for the different pallets.

Try the following to test for macro capability:

IF [ 4 GT 1 ] GOTO 100
M00

N 100
M00

If there is an error it probably means you do not have macros functional.
Note: the square brackets around 4 GT 1, these are not parens () because parens are used for comments. And they are not {}, at least on HAAS.


In your machine is it possible to address a variable with an ahphanumeric label? You used the assignment PL = 1 where I might expect that you would have use the #number for a variable address. Thus, instead of
PL = 1
I have to use for example
#100 = 1
on a HAAS machine.

In a previous post of mine I referenced the variable #3028. I believe this is a HAAS variable that they automatically load with the number of the pallet in the station. If this is the case, then you would not need to manually load the pallet number. Rather you would simply use a test on #3028 to determine your action.

At this point we really need to know whether you have macro capability.

If you do not have macros you may not be able to load values into variables except as allowed thru G-code parameters where everthing in terms of internal storage is hidden from you.

.

Post what macro statements you wrote to get the errors and what the errors were. As Gar said as well, #3028 is a Haas variable. Your machine may use a different variable for pallet number.

And yes, you could alter my example slightly and get it to work on your machine by using other methods. Block skipping is one way. Do you have multi-skip? If so, then you could do this:

/N100
/G10L20P1X??Y??Z??B??(G54.1 P1 FOR PALLET 1)
/G10L20P2X??Y??Z??B??(G54.1 P2 FOR PALLET 1)
/G10L20P3X??Y??Z??B??(G54.1 P3 FOR PALLET 1)
/G10L20P4X??Y??Z??B??(G54.1 P4 FOR PALLET 1)
/G10L20P5X??Y??Z??B??(G54.1 P5 FOR PALLET 1)
/G10L20P6X??Y??Z??B??(G54.1 P6 FOR PALLET 1)
/GOTO300

/2N200
/2G10L20P1X??Y??Z??B??(G54.1 P1 FOR PALLET 2)
/2G10L20P2X??Y??Z??B??(G54.1 P2 FOR PALLET 2)
/2G10L20P3X??Y??Z??B??(G54.1 P3 FOR PALLET 2)
/2G10L20P4X??Y??Z??B??(G54.1 P4 FOR PALLET 2)
/2G10L20P5X??Y??Z??B??(G54.1 P5 FOR PALLET 2)
/2G10L20P6X??Y??Z??B??(G54.1 P6 FOR PALLET 2)
GOTO300

N300(START PROGRAM)
.
.

In this manner, you set block skip 1 to to ignore pallet one, or set block skip 2 on to ignore pallet two. This forces user input though. I prefer using a machine variable to identify the set up to eliminate the human input.

On your pallet is there one part, or is it a tombstone with many parts?
......
Try the following to test for macro capability:

IF [ 4 GT 1 ] GOTO 100
M00

N100
M00
One part (a casting) clamped in a fixture, no tombstone. The casting is not square.

Ill give the example a test when i get to work, thanks.


Post what macro statements you wrote to get the errors and what the errors were.
...
Do you have multi-skip?
....
I prefer using a machine variable to identify the set up to eliminate the human input.
A=2
IF[A EQ 2] G54.1 P21

Recived the same error message for both lines.
I'll have to post back the error, its on a peice of paper which i forgot at work.

Nope, no multi-skip block.

And we (me and the day guy) would agree, if we cant get the IF's to work, ill set up the G10 L2's for both pallets and we'll just delete the set we dont want to use during set-up.



_

060728-1332 EST USA

iMisspell:

Try the following:

My previous suggestion

IF [ 4 GT 1 ] GOTO 100
M00

N 100
M00

and then try this

#100 = 1

IF [ #100 GT 1 ] GOTO 100
M00

N 100
M00

See if either of these produce errors.

If these are error free, then we can discuss how you might handle the non-square casting.

.

Try what Gar suggested......

Also.....

A=2
IF[A EQ 2] G54.1 P21


This won't work like this. You need to do this:

#500=2
IF[#100EQ2]GOTO100
N100
G90G10L20P21X??Y??Z??B??(SETS G54.1 P21)
.
.
.
.

"A" is an argument setting attached to "#1". To set "A", you need to use it in a variable setting format like this:

G65P1234A2.

You could do this:

#1=2
IF[#1EQ2]GOTO100
N100
G90G10L20P21X??Y??Z??B??(SETS G54.1 P21)


But I wouldn't use local variables this way. I'd set it to a common variable like #500 and above. Most machines on reset, will dump values in the local variables and even commons 100. This would cause a problem if you had to restart a program since now your value is "0" or null.

060728-1554 EST USA

psychomill:

You may have a typo.

I think you meant

#500=2
IF [#500 EQ 2] GOTO 100

.

Thanks Gar..... :cheers:

Ok...

This worked fine...
IF[4 GT 1] GOTO ###

And this also worked fine...
#123 = 2

When i tried ...
A=1 (the other night)
and
IF[4 GT 1] G54.1 P21 (tried this tonight)

Recived 114 - FORMAT ERROR IN MACRO for each line.

Thats all the time i had to play with that stuff.
Was gonna try IF [#123 EQ 2] GOTO ### but got side tracked and forgot, will try on monday.

Did use G10 L20 P#1-5 at the top of the program and it worked great, really hope the day guy digs this. Would be nice to save the current work and tool offsets to a file (gonna start a new thread (http://www.cnczone.com/forums/showthread.php?t=22928) about this) for reloading next time.

Like i said earlyer, im new to this machine, after peek around alittle more and talking with the day guy alittle more (tring to get clear answers from him), pre-part he uses the same offset numbers for each pallet (as of now ive only been using one pallet), the reason for the two sets of work offsets P0# and P2# is so they can set up a job on pallet A and set up a different job on pallet B and not have to mess with anything after that and some where along the lines they where gonna run the same part on both pallets so there was no down time during a part change but somthing happened with that whent out the window... at times i just get frustreated at how they place operates and im like whatever and stop asking questions of why :)

So with that said :) no reason for the IF statments any more. BUT im glad i asked about them, learned quit a bit in this one thread and im sure there will be a time where it will help.
Setting the G10 L20 P0# at the beginning of the edited programs will be just fine and work well, but more ideas are wellcome :)

Thanks again for all the help and explanations, been a big help.


"A" is an argument setting attached to "#1". To set "A", you need to use it in a variable setting format like this: Just read abuot this in another thread, gonna have to see if i can find the book for the machine to see a listing of all the varable settings.


If these are error free, then we can discuss how you might handle the non-square casting.Like i said earlyer, my hands are kind of tied with the amount and degree of changes i can make, but i deffinitly would like to hear what your thouhgts are about this, if you fell like sharing.


_

I have done this many times in fanuc controls, and I've developed a different approach:

O0001;
(PALLET 1 DRIVING PROGRAM);
#1=0;
#2=1;
M98P0003;
M99;

O0002;
(PALLET 2 DRIVING PROGRAM);
#1=10;
#2=1;
M98P0003;
M99;

O0003;
(PART PROGRAM);
IF[#2EQ0]GOTO9998

M6T1;
G90 G00 G54.1 P[1+#1] X0 Y0 S1000 M3;
...
...
...
G90 G00 G54.1 P[2+#1] X0 Y0 S1000 M3;
...
...
...
G90 G00 G54.1 P[3+#1] X0 Y0 S1000 M3;
...
...
...
G90 G00 G54.1 P[4+#1] X0 Y0 S1000 M3;
...
...
...
GOTO9999;
N9998 #3000=1(PALLET NOT ASSIGNED);
N9999M30;





Variable #1 stores the value to be added to P in the G54.1P# line.
This means that if you run program O0001, #1=0 so G54.1 P[3+#1] is the same as G54.1 P3
But if you run program O0002, #1=10 so G54.1 P[3+#1] is the same as G54.1 P13
Variable #2 is for error checking. Any time the machine is reset, or a program ends both #1 and #2 will return to zero. At the top of the part program we check to see that #2 does not equal zero. If it does, the program jumps to N9998. #3000 generates an alarm and stops the machine. This ensures that either program 0001 or 0002 was executed.


I've made several different variations of this. Which one is best depends on the exact circumstances, but this works pretty well in most cases.

Good luck!

060729-0915 EST USA

iMisspell:

Your experiments proved that:

(1) You have macro capability because no alarm on
IF[4 GT 1] GOTO 100
and/or
#123 = 2

(2) That your version can not understand the instruction
IF[4 GT 1] G54.1 P21

You did not test it but
IF [#100 NE 1] GOTO 300
G54.1 P21
GOTO 500

N300 ...

N500 ...

should work.


If G52 is all zeros (probably default on start of program on Fanuc), then
the command
G54
will place your work zero X, Y, Z, ... at a point in machine space offset by the contents of the G54 X, Y, Z, ... values relative to the machine absolute zero position (probably identified by the term MACHINE ZERO). Now any absolute moves will be referenced from the this G54 work zero (current work offset). This work zero can be anywhere you want relative to the physical part by your selection of the values stored in G54. This is a point in space relative to the machine frame and not the part. It is only referenced to the part by how you locate the part relative to the machine frame.

If G54 is left unchanged, and you move your part from the physical position where you defined G54 for your program, then the part will be machined incorrectly. This could be the case where you have two pallets and they clamp differently in the machine. In this case I like G52 because I can define G54 for one pallet, and use G52 for correcting the difference between the two pallets. This results in small difference values rather than two different G5xs with large values. Large values are always more error prone than small ones.

If you google with the search string

site:www.cnczone.com G52 gar

then you will find some of mine and others discussions on G52. The term "site:" before the web address limits Google's search to only that web address. This search method works better than the cnczone search. If you used the cnczone search for G52 the result is nothing.

You may find some information on my web sites useful. These are mostly not programming related.
www.beta-a2.com
www.beta-aa.com

(edit 060729-1030)
A manual that may be useful is the HAAS mill manual. Many functions and addresses are identical or similar to Fanuc. This manual is online as follows:

www.haascnc.com
click on CUSTOMER SERVICE
click on MANUAL UPDATES
click on OPERATOR's MANUALS
under heading OPERATOR's MANUALS
may have to wait
click on MID-96-8000
The download file is 12 megabytes.

MACROS are discussed at p87 in Adobe reader and HAAS p 81.
Variables are listed at Adobe p91 and HAAS p84.

The HAAS manual is probably far more readable than a Fanuc manual.

You might want a HAAS control after you find out how easy it is to work with.
(end edit)

.

Thanks for your input, wmyerscnc.

... A manual that may be useful is the HAAS mill manual. Many functions and addresses are identical or similar to Fanuc. This manual is online as follows:.... Thanks, an earlyer google search brought me to an older HAAS manul, thanks for an up-to-date one.
I did a quick search for a Fanuc 16i control but couldnt find anything, ill have to search for it at the shop and make copys ...

_