Dialog4 Parameter Programming Question

Anyone here know if you can use Parameter formulas/calculations, in blocks between G41/G42 (start of tool compensation) and G40 (end of tool compensation? I know you can use simple parameters inside those blocks, but am having issues with formulas that are written inside tool compensation blocks.

Not seeing any discussion of this in the Dialog4 parameter manual and none of the examples show formulas inside tool comp, only in blocks before or after tool comp.

Don't have an answer, sorry. Eons since i used the Parameter programming features....CAM system sort of negated the need.
Believe that there are features of the parameter programming that don't appear in the supplemental programming manual.

Some time back Martin posted about features that were not in the manual.Things he picked from Euro forums...ways to enter different values in different locations within a block .
Might do a search to see if anything there has value for your question.

See: https://www.practicalmachinist.com/...oblem-109312/?highlight=Parameter+Programming

Would like to see your code....

On edit, just looked at the "software Update" booklet for Dialog 4 and within the section on parameter programming there are examples of calling "P" values within a compensated (G41/G42) moves....
(programming example #3 page 1-32)

Looks to be compound "P" values used there with math operations ...Did not spend too much time with this, but looks like the pocket is cut with a tapered wall where the cutter path is changed as it steps down,
Sort of cute...
Cheers Ross

$%9998

t1 r0.0625 a l a

p1 =1.0
p2 =0
p3 =0
p4 =((p1:2):0.86602)
p200 =(p2+p5*p4)
p300 =(p3+p6*p4)



%
($%9998/000000"hex via parameter)
n1 g17 t1
n2 z1 f35.0 s+1250
n3 g0 x0 y0 c0
n4 z0.1 f10.0
n5 p5==0.5
n6 p6==-0.8660
n7 x= p200 y= p300
n8 p5==-0.5
n9 p6==-0.8660
n10 x= p200 y= p300
n11 p5==-0.8660
n12 p6==0
n13 x= p200 y= p300
n14 p5==-0.5
n15 p6==0.8660
n16 x= p200 y= p300
n17 p5==0.5
n18 p6==0.8660
n19 x= p200 y= p300
n20 p5==0.8660
n21 p6==0
n22 x= p200 y= p300
n23 p5==0.5
n24 p6==-0.8660
n25 x= p200 y= p300
n27 g0 z1
n28 m30
?
0000

Something happened to my formatting when I pasted this into the forum- all the letters changed from upper case to lower case.
Program runs perfectly on my FP4NC, when I try to add tool compensation via G41/G42 I get error messages and it won't run.

This is a program to machine a hex- "P1" is the inscribed circle of the hex flats.
We use "P" values with compensation on (and also inside canned cycles) every day, the issue here is "calculations/formulas" inside compensation.
Would like to run tool comp to adjust the finished size of the hex and also apply G7 to the outside corners.
Tool comp would also allow this program to make either internal or external hexes just by changing which side of the hex the tool is on via G41 or G42.

Steve:
Funny, but i wrote this hex milling program some years back....bit of digging and this is what i have on this.

N1 G0 X0.0 Y0.0 Z4.0
N2 G17 T1*1
N3 S= P6
N4 G0 Z.1 M70
N5 G91 Z = -P13 F= P4 M70
N6 G90 M70
N7 G41 G47 A= P7 X= P10 Y= -P11 G0 G64 G61
N8 X= -P10 F = P5
N9 G7 R= P12
N10 X = -P9 Y 0.0
N11 G7 R = P12
N12 X= -P10 Y= P11
N13 G7 R= P12
N14 X= P10
N15 G7 R= P12
N16 X= P9 Y 0.0
N17 G7 R= P12
N18 X= P10 Y= -P11
N19 G7 R= P12
N20 X 0.0
N21 G40 G47
N22 G91
N23 G0 Z.1
N24 G90
N25 L= P14 N5 N24
N26 G0 Z.1
N27 T1
N28 L1 N5 N26
N29 G0 Z4.0
N30 G0 X0.0 Y0.0
N31 M30




P list (mode 12)

P1= (Hex size , across flats given in inches)
P2= (Height of hex in inches)
P3= (number of depth passes to get full height)
P4= (feed rate for depth moves) Note: rate will be 1/10 of value entered here
P5= (Feed rate around profile) Note: rate will be 1/10 of feed rate entered here
P6= (+Spindle speed)
P7= (enter value for arc out and arc into contour)
P9= P1* .5774
P10= (P1*.5774) / 2
P11= P1 / 2
P12= P1 / 8 (this setting makes the corner radius as a percent of the hex size, shown as 1/8 the hex size here)
P13= (P2 / P3) + .100
P14= P3 - 1

Some explanation:
P1 is the size of the hex you wish.
P2 is eh height of the hex.
P3 is the number of cuts needed around the profile to get to full depth.

The program cuts the profile to depth then calls a finish tool for final passes around the part.
Hex is oriented with the starting flat parallel with the "X" axis)
Corner radius is a function of the hex size...can set that amount in "P" 12.
Profile cuts are retracted at the end of the profile before reposition and next depth cut.
Depth moves are done incrementally, so it might be possible to have accumulating errors if lots of passes are needed to get the depth...

As with anything, might be errors in typing this so proof the program and use at your own risk..

T1*1 is the rough cutting tool. Call cutter radius larger than the true size of the tool by the amount needed for finish cut.
T1 is the true size (radius) of the tool.
Both rough and finish cuts done with the same actual tool.

Cheers Ross

Too funny, I got the idea from reading one of your old posts!
I was able to get this to work, simply a matter of getting G41/G42 in the correct block, in this case, following N4.
Will cut internal or external hex, depending on whether G41 or G42 is used.
Thanks for the follow up-cheers!