Mastercam X3 Work Coodinate Help ?'s

[wildcatmahone]

Hey All,

New Mastercam user here with a couple questions regarding the code I'm receiving after post processing. Machine is a Chinese 4 axis VMC Fadal clone with Fanuc wannabe control. In the past I have been touching off stock on the XYZ and using G54-G59 work coordinates and running whatever part. After processing my first code today I am not getting any G54's etc in the processed code just an "e" where I think the G54 should be. If anyone knows please explain this "e" in the code to me and how to use it and if I need to make any changes in the CAM parameters.

Question 2:
After a M06 code the machine runs into its own locked tool change subprogram any modifications need to be made in the machine definition file for the tool change to work properly? What's a forced tool change?

Question 3:
In the operation manager tool setup menu I see it give you the option of specifying tool holder diameter and bore, tool length diameter shoulder length flutes etc.
Does changing the tool length in this menu have any effect on the final code or is it just for reference. I am touching off tools on the part using negative offsets and don't need any spindle crashes. Hope this makes sense and Thx in advance.

[Superman]

... today I am not getting any G54's etc in the processed code just an "e" where I think the G54 should be. If anyone knows please explain this "e" in the code to me and how to use it and if I need to make any changes in the CAM parameters.
e is not normal output, I think the post has been editted and a $ is omitted on 1 line, the X family of posts require postblock outputs to end with a ,e$
I would guess the "pwcs" area would be a starting point

Question 2:
After a M06 code the machine runs into its own locked tool change subprogram any modifications need to be made in the machine definition file for the tool change to work properly? What's a forced tool change?
Is M6 the code the machine needs to do a toolchange ?
If your machine uses a different code, then the call-up in the post should be altered
Force tool change is used to reset items, or return to the toolchange point. The post may need to be customised to your needs

Question 3:
In the operation manager tool setup menu I see it give you the option of specifying tool holder diameter and bore, tool length diameter shoulder length flutes etc.
Does changing the tool length in this menu have any effect on the final code or is it just for reference. I am touching off tools on the part using negative offsets and don't need any spindle crashes. Hope this makes sense and Thx in advance.
Mastercam uses the tool size values to calculate the toolpaths, the holder values are use in some operations for gouge aviodance, it uses these values also for backplot and verify. It is good practice to define the tool as accurately as possible ie tool length to show where the tool ends and holder starts while doing a deep pocket, if the tool goes below the top level then the holder has hit the part, a good programmer may omit the holder definition if he has good 3D visualization skills

[wildcatmahone]

Thx for the reply. Got to work more on setting up the X3 to suit these machines today and am making progress. Ran my first program via a flash drive through DNC mode and all appears to be running smoothly. Not too bad.

I was able to sort out the problem with the G54's not posting. I was running the Fadal machine definition which only had two work offset options G92 and the "E's" which I was having problems with as mentioned earlier. Never heard of these "E's" as an offset code before must be a new Fadal setup or something. Anyway, I used the generic 4X mill Fanuc setup instead today which had G92 or G54-etc as offset options and it worked out well. The machine was locating to the part and the ATC was working beautifully with the M6 call.

The only problem I caught was that the post was putting a M01 right before the tool change and this machine doesn't read M01's so was giving me an alarm, weird. So I had to edit the post changing the M01 to M00 which the control does read or I suppose I can delete it altogether as it's unnecessary. Is it possible to configure Mastercam to leave out these M01's to save me the hassle of editing the post each time, where would I do that?

Also, I am trying to measure out the tool lengths etc the best I can without a presetter to fill in the tool data in the tool definition files. What's the best way to configure a post using G43 and negative length compensation (touching off Z0 on top of the part).

One additional question, got a hollow vertical cylindrical cast part needs a simple bore from the top center but also requires a counterbore from inside the part. Any ideas how to machine a feature like this? Thanks for the previous advice.

[Superman]

The only problem I caught was that the post was putting a M01 right before the tool change and this machine doesn't read M01's so was giving me an alarm, weird. So I had to edit the post changing the M01 to M00 which the control does read or I suppose I can delete it altogether as it's unnecessary. Is it possible to configure Mastercam to leave out these M01's to save me the hassle of editing the post each time, where would I do that?

There should be a switch near the top of the post to disable the output of M01, 1=YES or ON, 0=NO or OFF

Also, I am trying to measure out the tool lengths etc the best I can without a presetter to fill in the tool data in the tool definition files. What's the best way to configure a post using G43 and negative length compensation (touching off Z0 on top of the part).

I use Okuma's, typically I activate the co-ord system on the machine, set a face as Z0 and bring the tool into contact with a gauge block ( tool setter or similar on the Z0 face ) and calculate this gap on the tool's length set page
I normally program the Z0 is the top of the part, any Z- is below the job and is capable of cutting material. Z+ is in the safe area

One additional question, got a hollow vertical cylindrical cast part needs a simple bore from the top center but also requires a counterbore from inside the part. Any ideas how to machine a feature like this? Thanks for the previous advice.

Draw this casting as a solid on it's own level, and select it as the "solid" on the "verify" set-up page, you can also select it as the stock in the "Stock set-up" in the Operations Manager

Interpolate the bore with a cutter, and do the same with the C'bore