[darrylh]

Seasons greetings to all.

I am new to CNC and have purchased an affordable software package called Kipware M. I am having a problem with getting the control to accept the cutter diamater information. This information is entered in Kipware but if I use a 4mm cutter - and specify either 4mm, 6mm or 8mm cutter in the software - I get the same shape every time and the y-axis dimension is always 4 mm less than it should be when I refer to my drawing. I figure the machine doesn't know anything about the cutter (and assumes the spindle centre line) or the software isn't uploading the details to the machine. At first, assuming the software brought in the cutter deatils to the control, I thought (being a newly-acquired machine) the 100-102 parameters might have the wrong multiplier for the y-axis - but it checked out perfectly when tested. I am specifying G40 in the software. Other than this glitch, the software suits my basic needs.
Can someone please advise me how a 4mm cutter can be manually written into the code, including an example syntax, and where in the order of code it should go. Some might say I should go back to the software authors but from previous support experience I doubt they will be able to give me an answer on the control side of things.
Best, Darryl

[Stu_M3]

Sound like your software is pumping out a centreline cutter path.To apply cutter compensation specify the cutter radius on the geometry offsets page of the control, I use G101 For tool1 G102 for tool 2 etc and keep G001-G099 for length offsets.G41 Is used to apply the offset. For example to machine an external profile of a square 100mm x 100mm 5mm deep with a 10mm cutter.

set G101 to 5.00
%
O1234
G54
G21
G17G40G80G90
G0G91G28Z0
M6T1
S2500M03
G90
G0X70.000 Y-70.000
G0G43Z50.000H1 (LENGTH OFFSET G001)
G01Z2.0F1500
Z-5.0
G41 Y-50.00 D101F500 (CUTTER COMP APPLIED HERE)
X-50.000
Y50.000
X50.000
Y-70.000
G40X70.0 (CUTTER COMP REMOVED)
G0Z100.000M05
G0G91G28Z0
M02
%

hope this sorts u out.
Stu

[BlueChip]

Darryl,

Being one of those authors ... we would certainly offer any support we can. Here are a couple of thoughts :

(1) If you are using one of the standard menus, the software automatically adjusts for the size of cutter entered when roughing ... and uses G41 / G42 for finishing. When G41 / G42 are used, the menu also asks for an "Offset Number", this comes out on the code as a D value. You then need to enter the actual radius of the tool in that offset number at the machine. For example, you entered offset number 32 in the field on the form, the code might say :
G01 G42 X---- Y---- D32 F20.0 ;
You will need to enter the radius of your tool in offset #32 at the control. This is the best way to program as you can easily adjust for dimensional differences due to cutting conditions or whatever by simplying adjusting your value in offset #32.

(2) If you have drawn your shape in the SketchPad and are then using the conversational roughing or finishing menu to describe your cutting conditions, you will need to select one of the G41 or G42 buttons to have the software output the cutter comp code ... and then follow the above.

Oftentimes, users do program the path for the center of the tool and choose no cutter comp.. We recommend that even if you do draw the toolpath as the centerline of the tool, you should still select and add cutter comp to the program as it gives you an easy way to adjust for cutting conditions / dimensional problems using the offset table on the machine.

So, after all that basically, the software, like all software I think, does not send any cutter comp information into the offset tables of the machine. It places the correct G code information in the program, but the user must also complete the cutter comp call and information by entering the correct cutter information at the control. One without the other doesn't work. The program can call offset #32, but if no value or the wrong value is manually entered, no good .... or the reverse.

I hope this answered your question. If not, please don't hesitate to re-post or contact me at my personal email at Kentech and I will be happy to lend any info I can. My email is kskonech at kentechinc.com.

[darrylh]

Thanks stu and bluechip for this help. The suggestions make total sense and I will try asap. I like Kipware M and was surprised how quickly I could get the CNC m/c cutting - having made very slow progress with a couple of other software packages. My only criticism would be directed to the manual and slide shows which leave a number of questions unanswered for a newcomer to CNC software. Both need to be more comprehensive and detailed. However, I am liking the Kipware experience more and more and want to progress to the lathe module.

A question for Bluechip.............. essentially the parts I am making are just roughed out of sheet, without a finishing prog. I simply uploaded the roughing prog to m/c and ran it - it worked great but assumed a tool centre line exactly as Stu observes. Although, this was created without the 'create main program' routine, I did assume that maybe there were setting in the latter that the m/c needed to know, so I created a main prog with just the roughing sub prog. Here, I found that some additional formatting from the software caused several 010 alarms on the control. These I found were mainly T and M codes that I edited out on the control - and once removed, I essentially got the same results as with the original 'raw' prog. I have to say despite referring to the help notes, I wasn't quite sure what some of the fields needed in the 'create main prog' (e.g. height offsets) and left them blank - having already specified things like safe rapid height/co-ords for top & bottom of workpiece, in the roughing menu. Any further guidance in the right direction would be greatly appreciated, and I'd be happy to assist you guys if you need a user on the ground to try out improvements or new developments.

Best,
Darryl

[BlueChip]

Hi Darryl,

I'm kind of assuming that you might be using the SketchPad to draw your toolpath, then using the SketchPad Roughing Menu to create the program. If so, here are some suggestions ... if not, please re-post and let me know which menu you are using to create the cutting program.

In the SketchPad Roughing Menu, there is a CUTTER COMPENSATION OPTIONS box with a number of user available options that need to be set. First, The G41 / G42 buttons need to be selected to tell the software on which side of the part the tool will be cutting ... this depends on climb or conventional milling and which direction you drew the toolpath in the SketchPad. Second, is the type of approach or approach direction. Here you want to select an option that makes a smooth approach into your cutting path. Also, here is where the software uses your cutter diameter to automatically make a big enough move to activate cutter comp without any overcutting alarms. Last is the OFFSET NUMBER ... this is the D value placed in the program ( as mentioned in my previous post ) and where you will need to manually enter the radius of your cutter before running the program.

If all this is done, you should see a G41 or G42 and D value in the program G code produced when you select CREATE PROGRAM. Thsi should be in the "raw" program and nothing further regarding cutter comp is done in the MAIN PROGRAM option.

To address your questions regarding the CREATE MAIN PROGRAM option :

(1) The Height Offset establishes the distance from the tip of the tool at the tool change position to the Z zero point on the part. As explained about cutter comp and that offset, the Height Offset allows you to easily adjust for any Z errors due to cutting conditions by simply adjusting the value in the Height Offset used for that tool ... H01, H02, etc.. This offset value, as mentioned, is the distance from the tip of the tool at tool change to the Z zero point on the part. Each tool should have a Height Offset number, usually it corresponds to the tool number ... T01 uses H01, T02 uses H02, etc..

In the program, the command is G43 Z--- H-- to activate the offset and now the machine knows where the Z zero is located for that tool. If you command Z1.000, the control knows that from the tip of the tool to Z zero is some dimension (stored in the offset table), and it can calculate other Z dimensions based on that value.

On the form, you would enter 01, 02 or whatever, and at the machine you would measure that distance for the tool and place that value in the offset table under 01, 02 or whatever number you used on the form for each tool.

Also, if the tool breaks, you replace the tool and measure the tool height and enter that value into the offset. No program changes need to be made becuase the program only sees H01 or whatever. Also, next time you run the job, the program doesn't change, you are just loading new offset values for the tools now loaded.

The rapid height and safe height asked in the forms simply tells the software the Z dimension it can use to rapid around the part.

Hope this helps. As before, please re-post or reach me at kskonech at kentechinc.com.

[darrylh]

Thank you. You are absolutely right with the assumption that I have used sketchpad, then the roughing menu to produce the prog. Yes, I selected the 'approach' so that the cutter would come in gently to the workpiece. I did also try G42 compensation, as the cutter was to the right of the workpiece running around CCW - but the code produced seemed to throw up a number of 010 alarms on the control, as pointed out in my earlier reply. However, I had a look at the menu/offset pages on the control and found these were ALL blank. I am now in the process of entering this data as suggested by Stu, earlier in the thread. I will thoroughly go through your advice also and thank you for the response. I will get back with the results in a few days once I am back to work. Seasons greetings.