Feed plane issues

Mike @ BC-MFG · December 20, 2007

I'm using X2 MR2 mill level 1 with the MPMASTER post which I updated with X2. I've just recently switched from V9 and I've been using mastercam for about ten years. The problem I'm having is that whenever I try to use any circle toolpaths it ignores my set feed plane and instead uses the retract plane. Has anyone else had this problem? Is there a fix?

December 20, 2007

Are you using a retract, make sure your retract and clearance are set to different values.

Mike @ BC-MFG · December 21, 2007

I'm not using a clearance just retract.

Programinator · December 21, 2007

Sorry Mike It seems as though you are the only one with this problem.

December 21, 2007

I'd be curious to see some code of what you want as compared to what you are actually getting

Programinator · December 22, 2007

ya mike give us some code!!

Mike @ BC-MFG · December 22, 2007

G1 Z-.5 <---- What Im getting

Z-.5 <---- What I want

December 22, 2007

Not enough information Mike

Can we see the entire snippet on of the circle mills and the settings you are trying to use?

If I am understanding what I think you are trying to do, I think this is the closest you are going to get Mike

code:

G00 G17 G90 G54 X-1.1785 Y.7806 S1426 M03

G43 H1 Z.25

Z-1.249

G94 G01 Z-1.25 F6.33

Y.8744

X-1.0847

G03 X-1.1785 Y.9681 I-.0938 J0.

Y.5931 I0. J-.1875

Y.9681 I0. J.1875

X-1.2722 Y.8744 I0. J-.0937

G01 X-1.1785

Y.7806

G00 Z.25

Mike @ BC-MFG · December 22, 2007

The your settings for your sample program must have been something like this.

Retract .25

Feed plane -1.249

Top of stock ***

Z depth -1.25

If thats the case then yes thats exactly what I'm trying to do, however my feed plane is being ignored and it wants to feed from my set retract point. But when I'm useing contour it works like it's suppose to. HELP!

December 22, 2007

This was what I used for settings, I also had my geometry at that depth

Circle mill functions more like drilling than it does contour, you'll need to remember that.

Mike @ BC-MFG · December 22, 2007

If you were to add depth of cuts that wouldn't work because your telling it that you only have .001 stock thickness. I shouldn't have to tell it I'm doing something that I'm not to accomplish a given task. I want an absolute retract of .25 and an absolute feed plane of Z-1.25 also an absolute depth of Z-1.25 With .25 rapid step downs. The point is, is that V9 works like it's suppose to, even the version X demo works like it's suppose to, but not the X2 MR2 that we payed good money for. Is there a glitch maybe? I feel like I'm getting the run around from our reseller.

Programinator · December 22, 2007

John,

Mike is right when you set the feed plane to a negative number it should output a rapid move down to that point before feeding. Which is real handy when doing stepdowns and cutting some mad cycle time off. If it works for him on other tool paths why will it not work on a circle. Problem is that i have not seen this complaint before and thats kind of weird. It must be some kind of bug.

Mike,

Have you tried an install on another pc?

Wonder if mr1 does the same thing?

Could it be a post problem?

I know your entering in the correct numbers in the correct fields because you have worked with mcam for a long time which narrows down operator error.

Its mcam for sure or some setting of some sort or the post.

But your right it should be outputting the rapid z moves for you.

December 22, 2007

quote:

John,

Mike is right

I do not have a previous version installed on this computer any longer however I do believe he is, I haven't had to create in anger for awhile and I seem to remember it should rapid to the retract plane above the feed plane then feed to the actual cutting depth depth. I have made several changes and it seems to only go the the feed plane as an absolute move.

I would go ahead and send that one into to QC, somewhere along the way that functionality seems to have been lost.

Moldmaker74 · December 22, 2007

quote:

I feel like I'm getting the run around from our reseller.

As a word of caution, you may want to keep your words sweet incase you have to eat them later.

December 22, 2007

Well, I just reinstalled X2 MR1 and then X2 MR1 SP1 and the functionality is the same as it is now.

Mike @ BC-MFG · December 22, 2007

Moldmaker74,

I would be so willing to eat more than just my words if this problem would just get solved.

This is not operator error. So if anyone knows of a patch or some kind of fix for this please let me know.

Mike @ BC-MFG · December 22, 2007

So John,

Mike @ BC-MFG · December 22, 2007

So John,

Does it rapid to your set (absolute) feed plane or is it ignoring it and using your retract value?

December 22, 2007

Regardless of setting INC or ABS I get the absolute value that is set in feed plane.

It "seems" the ABS/INC doesn't work on this dialog box. And it looks like it never has, I just installed V9 MR0105 :shiver:

And it behaves the same way.

So at this point there is no fix or patch.

Email QC to inquire as to if this is expected behavior and to request the change.

Programinator · December 22, 2007

I have not used the circlemill toolpath much so i have not noticed a problem. I will check it out on monday (yes i have to work on monday) and see.

Mike @ BC-MFG · December 23, 2007

Let me know first thing, thanks.

crazy^millman · December 23, 2007

Mike you paid good money for the ability to use something that is night and day from what V9 was. I just last week was helping someone with XMr1 and thought to myself WOW how much it changed from that to X2MR2. I can do things so much faster, quicker, and easier than I ever did in V9 that alone is worth the price. I do not know you, but have a hunch you are having major withdraw from V9. Give it some time and do not let a small problem you are having with something taint your whole thinking of X2MR2.

I have read this and use this feature all the time and they way you want to use it really makes no sense to me. You have your reasons, but I think you might try a different approach and you might get what you are looking for. I still did not see what you are getting for posted code. I also did not see what you got when you tried a different post.

Now if you want to accomplish this it can be done and is easily done. Like what you said here is a file on the FTP called MIKES_25_RAPIDS.MCX in the MX2 folder.

Here is the code:

code:

O2525 (25 RAPIDS)

(CUSTOMER - ADD CUSTOMER)

(PART # - Mike @ BC-MFG REV - )

(PROGRAMMER - RON

(PROGRAM NAME - 25 RAPIDS.NC)

(DATE - DEC-23-2007)

(TIME - 7:28 PM)

(T1 - 1/2 INCH FLAT ENDMILL - H1 - D1 - D0.5000")

G0 G17 G20 G40 G80 G90

T1 M06 (1/2 INCH FLAT ENDMILL)

(MAX - Z.25)

(MIN - Z-1.25)

G0 G54 X0. Y0. S3056 M3

G43 H1 Z.25

Z-.25 <---------------- RAPID .25

G94 G1 X.0625 Y.0625 F24.45

G3 X0. Y.125 I-.0625 J0.

Y-.125 I0. J-.125

Y.125 I0. J.125

X-.0625 Y.0625 I0. J-.0625

G1 X0. Y0.

G0 Z.25 <-------------- RAPID .25

Z-.5 <----------------- RAPID -.5

G1 X.0625 Y.0625

G3 X0. Y.125 I-.0625 J0.

Y-.125 I0. J-.125

Y.125 I0. J.125

X-.0625 Y.0625 I0. J-.0625

G1 X0. Y0.

G0 Z.25 <-------------- RAPID .25

Z-.75 <----------------- RAPID -.75

G1 X.0625 Y.0625

G3 X0. Y.125 I-.0625 J0.

Y-.125 I0. J-.125

Y.125 I0. J.125

X-.0625 Y.0625 I0. J-.0625

G1 X0. Y0.

G0 Z.25 <-------------- RAPID .25

Z-1. <----------------- RAPID -1.

G1 X.0625 Y.0625

G3 X0. Y.125 I-.0625 J0.

Y-.125 I0. J-.125

Y.125 I0. J.125

X-.0625 Y.0625 I0. J-.0625

G1 X0. Y0.

G0 Z.25 <----------------- RAPID .25

Z-1.2499 <---------------- RAPID -1.2499

G1 X.0625 Y.0625 Z-1.25

G3 X0. Y.125 I-.0625 J0.

Y-.125 I0. J-.125

Y.125 I0. J.125

X-.0625 Y.0625 I0. J-.0625

G1 X0. Y0.

G0 Z.25

X-1.4079 Y1.2101

Z-.25

G1 X-1.3454 Y1.2726

G3 X-1.4079 Y1.3351 I-.0625 J0.

Y1.0851 I0. J-.125

Y1.3351 I0. J.125

X-1.4704 Y1.2726 I0. J-.0625

G1 X-1.4079 Y1.2101

G0 Z.25

Z-.5

G1 X-1.3454 Y1.2726

G3 X-1.4079 Y1.3351 I-.0625 J0.

Y1.0851 I0. J-.125

Y1.3351 I0. J.125

X-1.4704 Y1.2726 I0. J-.0625

G1 X-1.4079 Y1.2101

G0 Z.25

Z-.75

G1 X-1.3454 Y1.2726

G3 X-1.4079 Y1.3351 I-.0625 J0.

Y1.0851 I0. J-.125

Y1.3351 I0. J.125

X-1.4704 Y1.2726 I0. J-.0625

G1 X-1.4079 Y1.2101

G0 Z.25

Z-1.

G1 X-1.3454 Y1.2726

G3 X-1.4079 Y1.3351 I-.0625 J0.

Y1.0851 I0. J-.125

Y1.3351 I0. J.125

X-1.4704 Y1.2726 I0. J-.0625

G1 X-1.4079 Y1.2101

G0 Z.25

Z-1.2499

G1 X-1.3454 Y1.2726 Z-1.25

G3 X-1.4079 Y1.3351 I-.0625 J0.

Y1.0851 I0. J-.125

Y1.3351 I0. J.125

X-1.4704 Y1.2726 I0. J-.0625

G1 X-1.4079 Y1.2101

G0 Z.25

X1.049 Y1.2883

Z-.25

G1 X1.1115 Y1.3508

G3 X1.049 Y1.4133 I-.0625 J0.

Y1.1633 I0. J-.125

Y1.4133 I0. J.125

X.9865 Y1.3508 I0. J-.0625

G1 X1.049 Y1.2883

G0 Z.25

Z-.5

G1 X1.1115 Y1.3508

G3 X1.049 Y1.4133 I-.0625 J0.

Y1.1633 I0. J-.125

Y1.4133 I0. J.125

X.9865 Y1.3508 I0. J-.0625

G1 X1.049 Y1.2883

G0 Z.25

Z-.75

G1 X1.1115 Y1.3508

G3 X1.049 Y1.4133 I-.0625 J0.

Y1.1633 I0. J-.125

Y1.4133 I0. J.125

X.9865 Y1.3508 I0. J-.0625

G1 X1.049 Y1.2883

G0 Z.25

Z-1.

G1 X1.1115 Y1.3508

G3 X1.049 Y1.4133 I-.0625 J0.

Y1.1633 I0. J-.125

Y1.4133 I0. J.125

X.9865 Y1.3508 I0. J-.0625

G1 X1.049 Y1.2883

G0 Z.25

Z-1.2499

G1 X1.1115 Y1.3508 Z-1.25

G3 X1.049 Y1.4133 I-.0625 J0.

Y1.1633 I0. J-.125

Y1.4133 I0. J.125

X.9865 Y1.3508 I0. J-.0625

G1 X1.049 Y1.2883

G0 Z.25

X1.5736 Y-.9708

Z-.25

G1 X1.6361 Y-.9083

G3 X1.5736 Y-.8458 I-.0625 J0.

Y-1.0958 I0. J-.125

Y-.8458 I0. J.125

X1.5111 Y-.9083 I0. J-.0625

G1 X1.5736 Y-.9708

G0 Z.25

Z-.5

G1 X1.6361 Y-.9083

G3 X1.5736 Y-.8458 I-.0625 J0.

Y-1.0958 I0. J-.125

Y-.8458 I0. J.125

X1.5111 Y-.9083 I0. J-.0625

G1 X1.5736 Y-.9708

G0 Z.25

Z-.75

G1 X1.6361 Y-.9083

G3 X1.5736 Y-.8458 I-.0625 J0.

Y-1.0958 I0. J-.125

Y-.8458 I0. J.125

X1.5111 Y-.9083 I0. J-.0625

G1 X1.5736 Y-.9708

G0 Z.25

Z-1.

G1 X1.6361 Y-.9083

G3 X1.5736 Y-.8458 I-.0625 J0.

Y-1.0958 I0. J-.125

Y-.8458 I0. J.125

X1.5111 Y-.9083 I0. J-.0625

G1 X1.5736 Y-.9708

G0 Z.25

Z-1.2499

G1 X1.6361 Y-.9083 Z-1.25

G3 X1.5736 Y-.8458 I-.0625 J0.

Y-1.0958 I0. J-.125

Y-.8458 I0. J.125

X1.5111 Y-.9083 I0. J-.0625

G1 X1.5736 Y-.9708

G0 Z.25

X-1.3205 Y-1.0076

Z-.25

G1 X-1.258 Y-.9451

G3 X-1.3205 Y-.8826 I-.0625 J0.

Y-1.1326 I0. J-.125

Y-.8826 I0. J.125

X-1.383 Y-.9451 I0. J-.0625

G1 X-1.3205 Y-1.0076

G0 Z.25

Z-.5

G1 X-1.258 Y-.9451

G3 X-1.3205 Y-.8826 I-.0625 J0.

Y-1.1326 I0. J-.125

Y-.8826 I0. J.125

X-1.383 Y-.9451 I0. J-.0625

G1 X-1.3205 Y-1.0076

G0 Z.25

Z-.75

G1 X-1.258 Y-.9451

G3 X-1.3205 Y-.8826 I-.0625 J0.

Y-1.1326 I0. J-.125

Y-.8826 I0. J.125

X-1.383 Y-.9451 I0. J-.0625

G1 X-1.3205 Y-1.0076

G0 Z.25

Z-1.

G1 X-1.258 Y-.9451

G3 X-1.3205 Y-.8826 I-.0625 J0.

Y-1.1326 I0. J-.125

Y-.8826 I0. J.125

X-1.383 Y-.9451 I0. J-.0625

G1 X-1.3205 Y-1.0076

G0 Z.25

Z-1.2499

G1 X-1.258 Y-.9451 Z-1.25

G3 X-1.3205 Y-.8826 I-.0625 J0.

Y-1.1326 I0. J-.125

Y-.8826 I0. J.125

X-1.383 Y-.9451 I0. J-.0625

G1 X-1.3205 Y-1.0076

G0 Z.25

M5

G91 G28 Z0.

G28 X0. Y0.

G90

M30

%

[ 12-23-2007, 10:49 PM: Message edited by: Crazy^Millman ]

crazy^millman · December 23, 2007

Mike here is a screen shot of what I did so others can see how to do the same thing with any toolpath.

quote:

I want an absolute retract of .25 and an absolute feed plane of Z-1.25 also an absolute depth of Z-1.25 With .25 rapid step downs.

code:

G0 Z.25

Z-1.2499 <----------- RAPID TO 1.2499

G1 X1.6361 Y-.9083 Z-1.25 <------------ FEED MOVE OF .0001

G3 X1.5736 Y-.8458 I-.0625 J0.

Y-1.0958 I0. J-.125

Y-.8458 I0. J.125

X1.5111 Y-.9083 I0. J-.0625

G1 X1.5736 Y-.9708

G0 Z.25 <--------- RAPID TO ABSOULTE OF .25

X-1.3205 Y-1.0076 <---------- RAPID TO POSITION

Z-.25 <------ RAPID DOWN TO -.25

Sorry the last cut is .0001 to feed down to the -1.25 so I know you will be pissed and ready to throw Mastercam out that window for that.

HTH

Programinator · December 24, 2007

Crazy^Millman,

Looks like you can get it to work that way. But IMO i think thats the wrong way to do it and it takes much longer. It should be able to be done the same way its done in contour or pocket.

Retract abs .1

Feedplane abs -1.0

Top of stock abs 0

Depth of cut abs -1.0

In depth cuts: Max step .25

Fin passes 0 (or the num of fin passes you want)

fin pass depth 0 (or how much you want to take off for fin pass)

To me thats the way mcam wants you to do it. To me thats the way it should be done. looks like to me your doing 5 rough passes and calling it fin passes.

I agree with Mike

Mike @ BC-MFG · December 24, 2007

Ok so it seems I'm not the only one who can't get it to work properly. Like I said earlier I refuse to lie to it, to get it to do what it should. This should be submitted to QC. Feel free to submit it to QC. I will too.

Shawn you've got it right, why are we the only who seem to care?

Sign In

Welcome to eMastercam

Feed plane issues

Recommended Posts

Link to comment

Share on other sites

Guest

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Guest

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Guest

Link to comment

Share on other sites

Link to comment

Share on other sites

Guest

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Guest

Link to comment

Share on other sites

Link to comment

Share on other sites

Guest

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Guest

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Link to comment

Share on other sites

Join the conversation

Recently Browsing 0 members

Join us!

Useful Links

Legal

Follow us