[Phishaholic]

I just got a used PCNC1100 first gen. I'm making few parts now. I'm a CNC Newb but getting the hang of it. The machine came with SheetCam and was upgraded to Mach3. I'm trying to make duplicate parts in a single cycle. the parts are simple 2.5D single tool parts. I know there is a way to do it, can it be done in Mach3? Second question, Of all of the CAM programs out there which ones seem to be the more user friendly ones? I'm running SolidWorks 2004 without too many issues. I'm pretty much self taught on that program.

Larry O

[Geof]

If I understand your question correctly you simply use one Work Coordinate system for one part and another for the the second.

You can do it by either duplicating the entire program and running through the first iteration using G54 and then use G55 for the second.

A more elegant way is to make your program a subprogram which you call after selecting G54 then call again after selecting G55 in the main program.

[Phishaholic]

Geof
First upfront thanks for the help! Second me being a Newb to CNC I will likely have questions for the group.

I like the second idea of a program with a subprogram. the program I'm running has 350+ lines unlike the 27 of my example. I think I have an understanding of the work offset table, you would put the origins for each part in the table and can call them up using G54 through G59 P254. I'm just not sure how to do the call outs for each in a program. If you would not mind can you modify my example. Thanks!!

Larry O

N0010 ( CUT A 1 INCH DIA. CIRCLE)
N0020 ( TOOL DIA. 0.125)
N0030 ( 2 STEPS @ 0.125 PER STEP )
N0040 ( TOTAL DEPTH OF 0.25 INCHES )
N0050 G0 G49 G40 G20 G17 G80 G50 G90
N0060 M6 T1
N0070 M3 S1200
N0080 M8
N0090 G00 Z0.35
N0100 G00 X1.2375 Y0.8
N0110 G00 Z0.1
N0120 G01 Z-0.125 F5
N0130 G03 X1.4375 Y1 R0.2 F10
N0140 G03 X0.5625 Y1 R0.4375
N0150 G03 X1.4375 Y1 R0.4375
N0160 G03 X1.2375 Y1.2 R0.2
N0170 G00 Z0.1
N0180 G00 X1.2375 Y0.8
N0190 G00 Z0.1
N0200 G01 Z-0.25 F5
N0210 G03 X1.4375 Y1 R0.2 F10
N0220 G03 X0.5625 Y1 R0.4375
N0230 G03 X1.4375 Y1 R0.4375
N0240 G03 X1.2375 Y1.2 R0.2
N0250 G00 Z1
N0260 M5 M9
N0270 M30

[Geof]

It will be something like this. I program on Haas machines and this is the way it would work on them. Mach may have some differences like the M97 P1000 may be M97 O1000 but the idea is the same.

O00000(This program selects the work zeros)
N0010 ( CUT A 1 INCH DIA. CIRCLE)
N0020 ( TOOL DIA. 0.125)
N0030 ( 2 STEPS @ 0.125 PER STEP )
N0040 ( TOTAL DEPTH OF 0.25 INCHES )
N0050 G0 G49 G40 G20 G17 G80 G50 G90
N0051 G54
N0052 M97 P1000 (This calls the circle program)
N0053 G55
N0054 M97 P1000 (Calls the circle program)
N0055 M5 M9
N0056 G91 G28 Z0.
N0057 M30
N0058 (=====)


O01000 (This cuts the circles_
N0060 M6 T1
N0070 M3 S1200
N0080 M8
N0090 G00 Z0.35
N0100 G00 X1.2375 Y0.8
N0110 G00 Z0.1
N0120 G01 Z-0.125 F5
N0130 G03 X1.4375 Y1 R0.2 F10
N0140 G03 X0.5625 Y1 R0.4375
N0150 G03 X1.4375 Y1 R0.4375
N0160 G03 X1.2375 Y1.2 R0.2
N0170 G00 Z0.1
N0180 G00 X1.2375 Y0.8
N0190 G00 Z0.1
N0200 G01 Z-0.25 F5
N0210 G03 X1.4375 Y1 R0.2 F10
N0220 G03 X0.5625 Y1 R0.4375
N0230 G03 X1.4375 Y1 R0.4375
N0240 G03 X1.2375 Y1.2 R0.2
N0250 G00 Z1
N0270 M99

[Phishaholic]

Geof
Thanks for the help. The Tormach uses M98 as callout for subroutines, I can see and understand the code now it makes sense.. I'm going to play and air cut a little tonight to see if I really get it. I would like to get a Haas Super Mini Mill when I graduate this machine if I can talk the wife into letting Me make an addition to the toolroom.

Larry O

[Phishaholic]

I'm not sure why its not working correctly. I have saved the work offsets in the table. The settings for Y and Z are the same for each offset and X is +3 from the previous offset. Basically it will cut the first two offsets and not the third.
Any thoughts would be nice.. Thanks!!

Larry O

O00000(This program selects the work zeros)
N0010 ( CUT A 1 INCH Square)
N0020 ( TOOL DIA. 0.125)
N0030 ( 2 STEPS @ 0.125 PER STEP )
N0040 ( TOTAL DEPTH OF 0.25 INCHES )
N0050 G00 G49 G40 G20 G17 G80 G50 G90 G41 G43
N0060 M6 T9 H9
N0070 M3 S1200
N0080 M8
N0090 G59 P10
N0950 G00 Y0 X0 Z1
N0100 M98 P1000 (This calls the Square program)
N0110 G59 P11
N0115 G00 Y0 X0 Z1
N0120 M98 P1000 (Calls the Square program)
N0130 G59 P12
N0135 G00 Y0 X0 Z1
N0140 M98 P1000 (This calls the Square program)
N0150 M5 M9
N0160 G40
N0170 M30
N0180 (=====)


O01000 (The Square Program)

N0210 G00 Z0.1
N0215 G00 Y0.5 X0
N0220 G01 Z-0.125 F5
N0230 G01 Y1 X0 F10
N0240 G01 Y1 X1
N0250 G01 Y0 X1
N0260 G01 Y0 X0
N0265 G01 y1 X0
N0266 G01 Z0.1
N0270 G00 Z0.35
N0280 M99

[Geof]

I can see nothing wrong in the program so you have me puzzled; double and triple check your offsets and calthem in a different order to see what happens.

[benji2505]

Does it cut the second offset twice or does it only cut the first two offsets once and then stop?

Benji

[Phishaholic]

Benji

It cuts the first two fine and the third one is kind of "D" shaped.

I have made a couple of changes to N0050 and N0060. They started off:
N0050 G00 G49 G40 G20 G17 G80 G50 G90 G41 G43
N0060 M6 T9 H9
And I changed it to this:
N0050 G00 G49 G40 G20 G17 G50 G90
N0060 M6 T9 G43 H9 G41
I did that because there was a couple of words from the same modal group on the same line. I also moved G43 because the manual said its better form to use it on the line with M6, But I will not check these changes until later today.

Another question I had was about the fixture offsets.
Is "N0090 G59 P10" the same as "N0090 G10 L2 P10 X10.278 Y-5 Z-10" the coordinates for the fixture are X10.278 Y-5 Z-10? Or would it be correct to write it like this"N0090 G59 P10 G10 L2"? I'm really not sure at this point. I'm going to do a little more air cutting and sharpie marker cutting this evening.

Anyone body with ideas at this point I'm pretty much open. Thanks!!

Larry O

[Geof]

If Mach works like most machines the G10 command just writes the coordinates into the offset register and you still need to call them. For example I can use G10 L2 G90 P2 X-8. Y-6. Z0. to put the coordinates -8. for X and -6. for Y into the G55 register on my Haas but I still have to use G55 to use that work zero.

Why do you use G59 P10, G59 P11, G59 P12, is that how Mach calls up offsets? I am used to just the single G54, G55, G56 etc.

[Phishaholic]

Geof

In this version of Mach for the Tormach you can use single work offsets like G54, G55, G56 etc. to G58, If you want to use any of the 250 others above that you use G59 P(and the number of the work offset) to call them out or G59 P1 is the same as G54. Getting ready to do a little air cutting and see if I can figure this out. I'll try changing the order of the call outs.

Larry O

[benji2505]

As described Geof, the G10 command only sets the x,y,z-values for the offset, but you still have to call the offset if you want to move there.

Generally speaking i do not think that your problem is related to the offsets though. Reason for this thought is that the first two runs are cut fine and you still move correctly to the third offset.

I have only guesses where the problem comes from: The G41 command usually requires a d-value and the value is assumed to be the defined diameter of the called tool if there is none. But the d-value can be overridden by a p-value for G41/G42. I could imagine that Mach starts choking on the P-values of your offsets (???).

If I was in your situation, I would use G54 through G56, program G41 with a d-value on a separate line and then see where I go with this.

Keep us informed

Benji

[Phishaholic]

benji

I haven't tried what you are talking about yet, when you use the G42/G43 The D word or P word is it the tool number or the actual dia.? Should I put it in the subroutine and turn it on at the beginning and turn it off at the end?

Thanks!!
Larry O

[benji2505]

Larry,

The D parameter addresses the diameter that is stored in your tool table.

The P parameter can address the tool diameter comp with a value, I do not know anything more because I never tried it.

If you have your requested FEM in Tool 9 position and all the measurements have been entered correctly in the tool table then it should look something like this:

All reset (G17 G40 G49 G90 etc.....)
....

t09 (usually prepares the ATC to reel to the tool required, here not really necessary)
M06 (tool change sequence)
G43 H9 (tool height comp for T9 on)
G41 D9 (tool diam comp for T9 on)

....

Why do you call G91 at the end of your program? If you call G91 ... z0.0 the cutter should not go anywhere. Let me know, maybe you know something that I don't.

Benji

[Phishaholic]

Well I think I'm almost there with this bit of code. it will cut four 1 inch squares, the work offsets are 2 colums 2rows with 2" between Y's and X's and the Z's are the same setting, this is the lower left corner and top surface of each work piece. The problem is the Z, It will air cut about a half an inch above the work piece. I'm having trouble getting it to zero. what is the best way to zero the fixtures Z. I was thinking spindle touching top surface with the 0 tool selected, I have tried using tool#1 which is my master tool height gauge as the selected tool and it didn't work. I'm open to Ideason the best way to establish zero for the fixture. Thanks!!

Larry O

O00000(This program selects the work zeros)
N0010 ( CUT A 1 INCH Square)
N0020 ( TOOL DIA. 0.313)
N0030 ( 1 STEP @ 0.125 PER STEP )
N0040 ( TOTAL DEPTH OF 0.125 INCHES )
N0050 G00 G49 G40 G20 G17 G50 G90 G80
N0060 M06 T06
N0065 G43
N0067 G41
N0070 M3 S1200
N0080 M8
N0090 G56
N0950 G00 Y0 X0 z0.1
N0100 M98 P1000 (This calls the Square program)
N0110 G57
N0115 G00 Y0 X0
N0120 M98 P1000 (Calls the Square program)
N0130 G58
N0135 G00 Y0 X0
N0140 M98 P1000 (This calls the Square program)
N0141 G59
N0142 G00 Y0 X0
N0143 M98 P1000 (This calls the Square program)
N0145 G00 Z1
N0150 M5 M9
N0160 G40
N0170 M30
N0180 (=====)


O01000 (The Square Program)

N0210 G00 Z0.1
N0215 G00 Y0.5 X0
N0220 G01 Z-0.125 F5
N0230 G01 Y1 X0 F10
N0240 G01 Y1 X1
N0250 G01 Y0 X1
N0260 G01 Y0 X0
N0265 G01 y1 X0
N0270 G00 Z0.1
N0280 M99
N0290

[benji2505]

Hi Larry,

Good news on Friday afternoon! You are getting closer.

1. Question: why is Z off by roughly 0.5 inch?
The G-Code looks good to me.
Could be your offset values, could be the difference in values for the cutters (t00 vs t06). Too eliminate all those intermediate influences, put T06 in the spindle, open the offset page, set the tool column to T06. Set the Work Offset column to G56. Then move down T06 to the zero-surface with a thin paper (chocolate wrap) in between, until the paper cannot be moved anymore. You are now .2 thou above the Surface. Hit touch (or whatever the button is at the offsets) for Z. The Z-value in the offset G56 should change. Repeat for all addressed offsets G57 ... G59, should go really quick (6 mouse clicks).

After cutting you can put in t00 cutter offset to t00, then G00 to Z=0. If t0 rams in to the fixture, you know that one of the measurements of t00 or t06 was off. (:nono: , joke!!)

2. Question: What is the best way of setting the height offsets?
There are more answers to this question than there are machinists in this world. My personal opinion: Measure a precise T0 with a height gauge, then follow the procedure in 1. for the other tools. In this case you just keep the Z height offset for G56 (or whatever) constant and hit the height offset touch button in the tool offset column. For me that was always the most precise way.

Have a fun weekend!

Benji

[justgary]

Larry -

On the Tormach it is not sufficient to use T06 only. Use T06 H06 to get the tool height out of the tool table. That should cure your Z offset issue, provided that your tool table is actually correct.

Regards,

- Just Gary

[Phishaholic]

Gary
I should have noticed that, I removed it earlier and forgot to put it back. I must have been looking at the code too much and just skipped over that. Thanks Benji and Gary for your help!!!

[LeeWay]

To me, Sheetcam is quite easy. Couldn't you simply nest these parts in Sheetcam and skip all the offsets? Put each different part on it's own layer and then you could cut only the ones you wanted.
Once you have a standard tool list loaded into Sheetcam, it goes blazingly fast to setup or change.

Just wondering why all the offsets unless you just want to learn those?

[benji2505]

BobCAD/CAM >10K (?)
Alibre/Sprutcam 2K
TurboCad/CAM 0.5K

Proofing that you can still program it by hand - priceless

:banana: