Deleting of individual parameters in clause

[andrejculk]

I work on machine »FADAL 4020«. When I want to erase only definite parameter in clause, I must erase whole clause. Is it possible, that only definite parameter in clause would erase?
E.g. in clause »G0 G90 G17 G1 X15 Y23 E18« want to erased only parameter »G1« and »E18«.
I don't know this otherwise, as if I erase whole clause and then insert new without former two parameters. I erase whole clause with key »delete« and then enter new:
»G90 G17 X15 Y2«.
I would like only to erase »G1« and »E18«, that I wouldn't have to write remaining clause once again.
Is this possible?

[Neal]

To erase any "word" type the word followed by a semi colon and press the enter key
I.E. G1; and press enter or E18; and press enter. If you want to modify a word then type the word as it is then a semicolon and then the corrected word I.E M30;M3 will change the M30 to an M3
Neal

[andrejculk]

Thank you for quick Answer. I will try this tomorrow. I have still one question.
If I write programm:

N1 G21
N2 L100
N3 G0 Z15 H5
N4 G1 Z-14.5 F2000
N5 G42 F150 Y-15 D5
N6 Y100
N7 X2.5
N8 Y-15
N9 G40 Y-20
N10 G0 Z15
N11 M17 (here find mistake)
N12 M30
N13 T5 M6
N14 S1000 M3
N15 G0 G17 G90 X-2.5 Y-20 E11
N16 G0 X-2.5 Y-20 E11
N17 L101
N18 G0 X-2.5 Y-20 E12
N19 L101
N20 G0 X-2.5 Y-20 E13
N21 L101
N22 G0 X-2.5 Y-20 E14
N23 L101
N24 G53 Z0
N25 G0 X260 Y230 Z0 E0 H0
N26 M2

Found me mistake in line 11, there, where finish subrutine (M17). What is in programme wrong?

[Neal]

Here is the corrected program. Note the placement of the G21 and the data on line N1:
N1 O22 (TEST PROGRAM
N2 L100
N3 G0 Z15 H5
N4 G1 Z-14.5 F2000
N5 G42 F150 Y-15 D5
N6 Y100
N7 X2.5
N8 Y-15
N9 G40 Y-20
N10 G0 Z15
N11 M17
N12 M30
N12.1 G21
N13 T5 M6
N14 S1000 M3
N15 G0 G17 G90 X-2.5 Y-20 E11
N16 G0 X-2.5 Y-20 E11
N17 L101
N18 G0 X-2.5 Y-20 E12
N19 L101
N20 G0 X-2.5 Y-20 E13
N21 L101
N22 G0 X-2.5 Y-20 E14
N23 L101
N24 G53 Z0
N25 G0 X260 Y230 Z0 E0 H0
N26 M2

Neal

[andrejculk]

Thank you again.

[andrejculk]

I have one question again.

N9 G8
N10 G42 Y-65.3 F800 D1
N11 Y33.7
N11.1 X10
N11.01 G0 Z5
N11.02 X13.4
N11.001 Y12
N11.02 G1 Z-6
N11.2 Y3
N11.3 X-5
N12 X9.4
N13 Y-25.3
N14 G40 Y-35.3
N15 G0 Z5.

If exsist the order, with which number of clauses again were without decimals?

N9 G8
N10 G42 Y-65.3 F800 D1
N11 Y33.7
N12 X10
N13 G0 Z5
N14 X13.4
N15 Y12
N16 G1 Z-6
N17 Y3
N18 X-5
N19 X9.4
N20 Y-25.3
N21 G40 Y-35.3
N22 G0 Z5.

[Neal]

your feed rate MUST have a decimal point. I recommend that you ALWAYS use the decimal point. That way you will always be right and won't have to remember which one need it and which don't. All will accept the decimal with the exception of the Zero Offset value in the survey.

Neal

[andrejculk]

Is maybe possible in cycle to change depth of drilling only on one coordinate?
N13 S3200 M3
N14 G17 G90 G0 X16.8723 Y-51.9277
N15 Z9.8 H13 M8
N16 G81 G99 X16.8723 Y-51.9277 Z-20.9 R09.8 F220.
N17 X44.1723 Y-32.0931
N18 X54.6 Y0.
N19 X44.1723 Y32.0931 (only here I want changed depth on Z-20.8)
N20 X16.8723 Y51.9277
N21 X-16.8723
N22 X-44.1723 Y32.0931
N23 X-54.6 Y0.
N24 X-44.1723 Y-32.0931
N25 X-16.8723 Y-51.9277
N26 G0 G80 Z9.8
N27 G0 G90 M5 M9
N28 G53 Z0

So if that with what kind of order to change depth of drilling on coordinate in clause N19 on Z -20.8, everywhere elsewhere let drills on Z -20.9.

[jbexplorer]

add z change after x y and M45


N19 X44.1723 Y32.0931 Z-20.8 M45 (only here I want changed depth on Z-20.8)
N20 X16.8723 Y51.9277 Z-2.09 M45

[andrejculk]

What mean G8?

N10* OPERATION 1: CONTOUR
N11* WORKGROUP
N12* TOOL 1: 4.5 ROUGH ENDMILL
N13S7500M3
N14G17G90G0X-25.4873Y22.6892
N15Z2.H1M8
N16G1Z-3.025F800.
N17G8 (why postprocessor here make G8?)
N18G42X-21.8508Y18.9725F500.D1
N19G2X-21.9552Y18.7176I-.1072J-.1049
N20G3X-23.7941Y17.7744I.0438J-2.3495
N21X-27.2902Y11.7191I23.7941J-17.7744
N22X-27.1876Y9.6549I2.1594J-.9273
N23G2X-27.3561Y9.4371I-.1312J-.0725
N24G1X-32.3931Y10.728
N25G0Z-3.225

What is differently, when is not G8 on clause N17?

[Neal]

G8 is telling the control to turn off the feed rate ramping at the end of each block. G9 tells the control to turn ON the ramping of the feed rate at the end of each block.

Neal

[andrejculk]

Originally Posted by Neal G8 is telling the control to turn off the feed rate ramping at the end of each block. G9 tells the control to turn ON the ramping of the feed rate at the end of each block. Neal

What of connection have G8 whit CRC (I think vhen is on beginning G8 or G9, or when I not use non of them)?