[Zakuhai]

Hello there,
I have a problem with programmming an outer back radius on Sinumerik. I allways get this error: Channel %1 block %2 danger of collision due to tool radius compensation

Here is what i found in the diagnostics book.

10 751 Channel %1 block %2 danger of collision due to tool radius compensation
Explanation
%1 = Channel number %2 = Block number
The ‘bottle neck detection’ (calculation of the intersection point of the following, corrected traversing blocks) was not able to calculate an intersection point for the overviewed number of traversing blocks, resulting in the risk that one of the equidistant paths will violate the workpiece contour.
Response Alarm display. Interface signals are set. NC Start inhibited.
Remedy: Check the part program and modify the program (if possible) such that inner corners with paths shorter than the compensation value are avoided. (Outer corners are not critical, since the equidistants are elongated or intermediate blocks are inserted so that an intersection point is always provided).
Program continuation by: Press the RESET key to clear the alarm. Restart part program.

I could completly understand if this happened while making an inner radius. But I am making an outer radius so there shoud be no problem. I even make another radius just like that on the front of the part only with a different tool.

The product is large bearing barrel. I have no problem making the front radius with an ISO tool but when I try to do the back one with a grooving tool it gives me this error. I regularly make theese barrels but up to now we used programming withous G41 and G42. I only wanted to write the program with the compesatios because it makes the programming of new parts far easier. So it it absolutly possible to physically make this part withouts using compensatios and there is no collision!

Here is the program part:

N580 T5 D2 S180
N590 X80 Z-85
N600 G1 G42 X76.78 Z-89.07 F1
N610 X75.18 Z-90.44 F0.2
N620 X72.04 Z-91.93
N630X75 F50
N640 Z-85
N650 X77.28 Z-85.88
N660 X75.54 Z-88.29
N670 G3 X 67.44 Z-91.35 CR=6
N680 G1 X80 F50
N690 G0 G40 X180 Z-90

First it gave me the error at N620. So i tried making the first cut straight (by deleting the N610) and now it gives me the same error at N600!
Funny thing is when I try it with G41 it works but the shape is obviously way off.
I am using GIMY type grooving tool with radius 2.5. I have specified the radius correctly and the position to be 8. I even tried changing the position to 3 or 9 with no effect. I also tried labeling the tool as different type (same that worked for the front radius) with no succes.

Thanks for your help.

[Superman]

N580 T5 D2 S180
N590 X80 Z-85
N600 G1 G42 X76.78 Z-89.07 F1
N610 X75.18 Z-90.44 F0.2
N620 X72.04 Z-91.93
N630X75 F50
N640 Z-85 <------ what's this
N650 X77.28 Z-85.88
N660 X75.54 Z-88.29
N670 G3 X 67.44 Z-91.35 CR=6
N680 G1 X80 F50
N690 G0 G40 X180 Z-90.

Read your code, take the Z values for example
starting at -89.07, then going to -91.93, then trying to go to -85.88

you may want the tool to move to these points, but not with comp active...it's coming back underneath itself, like doing under the barb of a fishhook

What value in D2 ? try setting to D2=0.....just to see what the tool movements are
Have you tried programming the toolpath to go thru the tool radius centre, so D2=0 when using a R2.5 full rad groover

[Zakuhai]

The prorgam is supposed to make a roughing cut first. Which is not in shape of a radius but simple 2 lines with G1. Than it comes back up to X83 and then back to starting position of the radius Z-85 so it can finish the conture with the radius using G3. The material I use is a rod diametr=83 but before the back radius is being done I cut the shape of the barrel into the diameter so at this point it is about 80mm. As you can see in block 630 is F50 which serves us insted of G0 because when we used G0 we had some problems with crashes during resetting the machine for difrent parts due to carelessness of the operators. So going G1 and max feed is safer since it requries the spindle to be operational. Do you think that not using G0 to move back up and into position could be the problem? Also the D2 is correction index in the machine's database. There is T 1-8 and every T can have up to 10 Ds. The D contains all the information about the tool including:
X and Z geometry
X and Z offset
Type of tool (roughing, grooving, parting...)
Position of tool 1 to 9 or 10 if you count drills
And ofcourse the tool radius

If I would not select any D I would get an error because the machine would not know what tool and where it is.

[Superman]

It's the tool movement between N620 to N640
- it is a triangular move where the previous move (N620) cuts through the middle of it...... this triangular move MUST be able to fit a 5.0mm circle ( R2.5 offset) that the control is able to compensate to EACH point
- if the control cannot adjust it's path between each point, before reaching the next compensated point, then you will get an error

try this ( cancel comp on retract, then restart it again when cutting )
N600 G1 G42 X76.78 Z-89.07 F1
N610 X75.18 Z-90.44 F0.2
N620 X72.04 Z-91.93
N630 G40 X78 F50
N640 Z-85
N650 G42 D2 X77.28 Z-85.88 F0.2


Personally, I use a CAM system to output the actual compensated path, & not use G41/G42 at all
- as soon as you start adjusting a program that uses comp, then, errors will show up quite regularly, for the most basic reasons ie forgot to double the X movement, not enough space for compensation to work etc.

[Zakuhai]

Thanks I will try that tomorrow. I hope that the tool won't hit the material while retracting back up. The manual for this type of machine says that when changing G40, G41 or G42 you should allways move in both X and Z. I have a premade "space" for this tool cut by TAG type parting tool that is only 5mm wide. So I cannot move in Z axis anywhere until I get above the diameter of the part. Hopefuly the machine won't mind that I try to cancel compensation and move only in X.
The CAM system would be nice. But unfortunalety it is way too expensive. My emloyer bought some basic cheapest bundle few years ago but than they realised they would need to buy the preset templates for each machine which cost insane money. So the SW is useless for me. There is one machine in in and we don't have that one...

[Zakuhai]

It worked! Thank you very much. Now it all works fine.

[Superman]

Some things to remember when using cutter comp on a lathe tool
- the toolpath is adjusted from the programmed path, when only doing tapers (angles) and radii, and also adjusting itself on the approach/departure points of these features
--- if facing, or straight diameter turning, it is not altered.

Caution
- If you cancel comp, then wish to retract in 1 axis only, WHILE it was the process of machining a taper or rad......then be aware that you can have movement on an axis, that you have not programmed any.
ie While doing a chamfer, & the tool is "still adjusted" to the angle, you program a X retract move with a cancel comp. You will have movement in the Z axis

[StergiosCNC]

Hello to everyone!

I just upgraded and using SolidCam2018...
On this version there is an option of ''fixture collision'' for protection.
In pocket operation fixture collision is disabled permanent.
In 3d iMachining operation its enabled at the beggining but as soon as i choose my tool, fixture collision is disabled again...
Is any solution you can give me??
Uploading an example video which shows the use of this option.

https://www.youtube.com/watch?v=CbbXgna1Kac


Awaiting for any help!!

Thank you.