[starvinmarvin]

I am trying out madCam and have a few questions but the biggest is this. Does madcam support cutter comp? Programmable lead ins with g41 when profiling?

Thanks for any help,

[svenakela]

MadCam doesn't make curves.

[starvinmarvin]

I am not sure what you mean? Long version please.

[svenakela]

MadCam doesn't make curves, MadCam make lines and the cutter will be on the line all the time. So there's no need for G41.

EDIT: Of course you can add a G41 in a post processor or in the G code-file, if you are sure that the tool path consists of a certain direction only.

[starvinmarvin]

Ewwwwwwww, don't like the idea of having to edit nc files after post processing. Not a deal killer, considering the price, but a real limitation!

Thank you for answering my question.

[svenakela]

Ewwwwwwww, don't like the idea of having to edit nc files after post processing. Not a deal killer, considering the price, but a real limitation!

Thank you for answering my question.

It's not a limitation as long as you don't have a machine controller from the middle ages that can't drip feed. Actually, I have never ever missed that as a feature. It's a 3D processing tool, not a profiling G code generator. Besides that I cut press fit pockets for bearings made with MadCam. If I can, you can.

[Dan B]

I've been the computer-aided machining manager at this company for over 20 years, and in all that time we have never had a post that included cutter comp. It hasn't been an issue for us.

Dan

[starvinmarvin]

I have only been programming and running cnc for 16 years but I can't imagine not having it as an option. It just saves so much time to be able to adjust an offset versus re-posting a program. Just my opinion, but arguing against programming with variables is crazy.

Anyway, I have another question regarding madCAM. When creating pocket paths it will randomly raise to the c/p before making the next step over. Adjusting the step over will change where and how often it will do this, sometimes it will just stay in the pocket until it is done. Am I doing something wrong? Pockets are just 2"x4"x.5" deep or so.

Most of my needs are 2-1/2 D and I understand this is more of a 3D program. I like Rhino and having the cam program embedded with the cad so am hoping this will fulfill my basic needs. Cnc precision job shop that does a lot of jigs and fixtures. Been machining mostly stone the last few years but just got a 12 year old Kitamura VMC and need to upgrade my 12 year old cad/cam program that doesn't like virtual XP in Win 7. No, I don't machine stone on my metal cutting equipment.

Again, thank you for all of your help with my questions.

[Dan B]

I suppose if you are doing a lot of 2-1/2 D work, then cutter comp would make sense. We mostly are doing 3, 3+2, and 5-axis. Lots of compound angle hole drilling too. For us it's not useful, but we have had the odd occasion when the operator writes a manual program, and in those scenarios they do include cutter comp if it's profiling work, AFAIK.

Can you post an example of the pocket problem? It might be easier to diagnose with your test case.

Dan

[starvinmarvin]

I seem to have answered my own question while getting something to post here. I modified the default tool tolerance of .003 to .0001 and it quit jumping around, much better. Now I want to modify a post processor but can't find where they are. I went with the default install on C drive. Have Win 7 64 bit. Can you tell me where to look or the file/folder names to look for?

Found it! It is with the cutter files in Program Data folder.

[Dan B]

Information on how to edit the posts is in the help file.

Dan

[starvinmarvin]

I did find it and read through it completely but couldn't find the files to modify. I did find them and have made some modifications but can't figure out the first line after a tool change.

If someone would be so kind, please help me with the first line after a tool change. I can't seem to get it and none of the other posts I looked at did what I want.

The code I am looking for is:

G0G43X1.Y0Z.1H2G55S4500M3
M8

XYZ coordinates, H and S are of course variables.
None of the posts I looked at used the *FIRST_MOVE* section so I am not sure how to use it, or if it is what I want. My effort at using it didn't work.

Yes, I want all of this on one line.

[Dan B]

See if this example might help:

//MadCAM_POST_2013-02-20 by Dan Bayn
*VERSION*
1.14
*FILE_NAME*
AV-Fadal
*FILE_EXTENSION*
cnc
*FILE_DEST*
c:\cnc-code\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
3
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*END_SECTION*
*CUSTOM_VARIABLES*
Fixture offset;fixture_offset;E1
*END_SECTION*
*FIRST_MOVE*
N"lnbr" G00"x""y""fixture_offset"S"speed"M3
N"lnbr" D"toolnr"H"toolnr""coolant_on""zhome"
N"lnbr" G00"zhome"
*END_SECTION*
*RAPID*
N"lnbr" G01"x""y""z"F7500
*END_SECTION*
*RAPID_APPROACH*
N"lnbr" "x""y""z"F7500
*END_SECTION*
*RAPID_RETRACT*
N"lnbr" G01"x""y""z"F7500
*END_SECTION*
*RAPID_FEED*
7500
*END_SECTION*
*TOOLCHANGE_TIME*
.33
*END_SECTION*
*APPROACH*
N"lnbr" G01"x""y""z"F"feedz"
*END_SECTION*
*FIRST_CUT*
N"lnbr" G01"x""y""z"F"feed"
*END_SECTION*
*CUT*
N"lnbr" "x""y""z"
*END_SECTION*
*TOOL_CHANGE*
N"lnbr" T"toolnr"M6 (TOOL CHANGE: "toolname")
*END_SECTION*
*TOOLPATH_CHANGE*
N"lnbr" ( TOOL #"toolnr" CONTINUES)
*END_SECTION*
*TOOL_STOP*
N"lnbr" M5
N"lnbr" M9
*END_SECTION*
*PROGRAM_START*
%
(This code is from madCAM for the Fadal)
(Confirm path: This is path #"pgmnr")
N"lnbr" G0G17G40G80G90M5M9H0Z0
*END_SECTION*
*PROGRAM_END*
N"lnbr" G90G0H0Z0
N"lnbr" M30
%
*END_SECTION*
*LINE_START_NUMBER*
1
*END_SECTION*
*COOLANT_ON*
M8
*END_SECTION*
*COOLANT_OFF*
M9
*END_SECTION*

Dan

[starvinmarvin]

Thanks Dan,

I made the changes and this is the code that posted with the madCAM post below. I have attached the simple cad model with I hope the madCAM info. The blank line should have the M8 command. I have to get to get some work done so I will continue playing with this tomorrow, while running my router.

Thanks again for all of your help!

O1
G0G17G40G49G52G80G90H0Z0M11
G0G49G52Z0
T1M06(Roughing_FLAT_END_0,25)
G0G43 X3.5512 Y1.5550 Z0.1250 H1G55S4000M03

G1 Z-0.5000 F30
X1.4488 F30
X1.4450 Y1.5538




//MadCAM_POST_2003-12-10
*VERSION*
1.0_031210
*FILE_NAME*
Kitamura
*FILE_EXTENSION*
nc
*FILE_DEST*
c:\postfiles\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
4
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*CUSTOM_VARIABLES*
Fixture offset;fixture_offset;G55
*END_SECTION*
*FIRST MOVE*
G0G43 "x" "y" "zhome" H"toolnr""fixture_offset"S"speed"M03
"coolant_on"
*END_SECTION*
*RAPID_FEED*
10000
*TOOLCHANGE_TIME*
02.
*RAPID*
G0 "x" "y" "z"
*END_SECTION*
*RAPID_APPROACH*
"x" "y" "z"
*END_SECTION*
*RAPID_RETRACT*
G0 "x" "y" "z"
*END_SECTION*
*APPROACH*
G1 "x" "y" "z" F"feedz"
*END_SECTION*
*FIRST_CUT*
"x" "y" "z" F"feed"
*END_SECTION*
*CUT*
"x" "y" "z"
*END_SECTION*
*TOOL_STOP*
M5
M9
*END_SECTION*
*TOOL_CHANGE*
G0G49G52Z0
T"toolnr"M06("toolname")
*END_SECTION*
*TOOL_STOP*
M5
*END_SECTION*
*PROGRAM_START*
%
O"pgmnr"
G0G17G40G49G52G80G90H0Z0M11
*END_SECTION*
*PROGRAM_END*
G0G52X-10.Y0Z0H0
M30
%
*END_SECTION*
*LINE_START_NUMBER*
0
*COOLANT_ON*
M8
*END_SECTION*
*COOLANT_OFF*
M9
*END_SECTION*

[svenakela]

I want to jump back to the cutter comp problem. Thing is, this is a 3D toolpath generator and the 2.5D features are more kind of "nice to have". Like I wrote before it is not a profiling tool. Like I also wrote you can make your own processor that includes a G41 if you are certain that your tool paths are correct. Of course you have to edit the g file afterwards, or how are you going to change the cutter comp?..
When it comes to 3D it doesn't matter and it is the same in all CAM tools I've used.
Being a programmer or not - variables are only good if there's a use for them.

I have strong feeling you haven't changed your template settings as well, have you?
If you haven't it is described several times. Search this forum after template.

[starvinmarvin]

I acknowledged that this is a 3D program with some 2.5D capabilities. Since my main work is 2.5D I just wish it supported this type of work a little better. What is driving my interest in madCAM is it's tight integration with Rhino and price. Quite often I need to hold tenths tolerances so I use cutter comp all of the time.

No I had not changed the template settings but this morning I did change the mesh and units settings in Rhino properties. Is this what you are asking or is there more? I did do some searches but even "madcam template" was pretty broad.

[svenakela]

...

No I had not changed the template settings but this morning I did change the mesh and units settings in Rhino properties. Is this what you are asking or is there more? I did do some searches but even "madcam template" was pretty broad.

Open an empty file and change the settings according to the help file (they are per file basis).
Overwrite your favorite template by saving the empty file to the same name and location as the templates.
Now, next time you create a new file from the template your settings will already be there.