Mastercam 2018 Not assuming incremental dimensions on drill

[Amsha]

I trying using drill toolpath with incremental dimensions but its not working .

Se it :

  

And my program outputs like this:

.....

G81 X0 Y0 Z-3 R0 F50.

instead of this:

G81 X0 Y0 Z-5 R0 F50.

 

I analise the nci  file and the "-3" is there istead of -5. 

I try Mastercam 2019 and the same problem, even with another Post and machine. 

Cam someone know how to correct it? 

 

 

[Guest]

Are you expecting incremental output?

Those values are only incremental input....the distances are related to the position of the geometry chosen...

If you're looking for inc output, try changing Misc int # 2 to 1

 

[Amsha]

No. I just wont that mastercam calculate the real value, not incremental. If you work with 5 axis, you pick z value of a face and you wont drill a hole of  30mm deep, you put incremental of -30.mm, istead of calculating the value, last time i worked that way it was on Mastercam X7 to X9 and works fine.

 

[Guest]

I would send that in to your reseller

[Goldorak]

I assumed that your entity is drawn a -2.000 from the Z0 plane, so be sure to be in 3D mode when selecting your drill points 

 

if you selected them in 2D and de Z dept is set at 0.000, your G-code is correct 

 

if evreything is OK then is probably a post issue 

[Amsha]

AS Goldorak said , using the 2D/3D mode wouild correct the problem, i tested and it dosen´t. 

After test various ways i found that mastercam hangs on z value of the point selected, even if you change the value o "Top of stock..." it ignors. 

Look this exemple: 

I selected a point with the z coordinate value of 100.00 mm, configure the toolpath (drill) like this:

  

and i get this :

G98 G81 Z98. R2. F100.

Looks like Mastercam is ignoring the Value of "Top of Stock" .
Can someone test?

Drill_point.mcam

[nickbe10]

On ‎6‎/‎15‎/‎2018 at 7:14 AM, Amsha said:

I analise the nci  file and the "-3" is there istead of -5. 

Have you edited the post, CD or MD ?

[Amsha]

On 19/06/2018 at 9:42 PM, nickbe10 said:

Have you edited the post, CD or MD ?

CD or MD, translate please.

 

[nickbe10]

8 hours ago, Amsha said:

CD or MD, translate please.

CD = Control Definition   MD = Machine Definition

 

[Colin Gilchrist]

On ‎6‎/‎18‎/‎2018 at 4:54 AM, Amsha said:

AS Goldorak said , using the 2D/3D mode wouild correct the problem, i tested and it dosen´t. 

After test various ways i found that mastercam hangs on z value of the point selected, even if you change the value o "Top of stock..." it ignors. 

Look this exemple: 

I selected a point with the z coordinate value of 100.00 mm, configure the toolpath (drill) like this:

  

and i get this :

G98 G81 Z98. R2. F100.

Looks like Mastercam is ignoring the Value of "Top of Stock" .
Can someone test?

Drill_point.mcam

What you are attempting to do with your example makes zero sense. That is the reason it isn't working for you.

You can absolutely use the "Absolute" radio button option with the Drill Cycles, to force the system to ignore the "depth" of the Point.

Your problem though, is that you can't have a Top of Stock (TOS), that is "physically below" your geometry point, unless you also use the "Absolute" option to also override the depth of the drilled point, and that overridden depth is lower than your overridden TOS.

1. Your point is a Z100. (above Z Zero!!!)
2. You are then telling the system to "override" that TOS depth value, with an absolute value of Z0.0.
3. Then, you want to drill to "-2.0", Incremental, which is defined as an incremental distance, from wherever the geometry depth is located! This is why you are getting (correctly) a Z98. (Because your geometry is located at Z100.)
4. Your Top of Stock can never be defined as "below" the final drill position. Any time you attempt to do this inside Mastercam, the system wisely ignores your input, since it makes no logical sense.

To prove this to yourself, try entering a Top of Stock value of "105." absolute. You will get an "initial point" that is output before the G81 drill cycle. Also, try entering a Top of Stock as "5.0 Incremental". This will also work.

 

 

 

[Colin Gilchrist]

If you are defining Drill Points for a 5 Axis, I would highly recommend that you create a Point entity, at the actual top of your hole, and that you use Incremental for all your Clearance, Retract, Top of Stock, and Depth values.

Why?

Why would I recommend that you use all "Incremental" settings?

Because the depth values come from the "point" itself, relative to your Tool Plane and WCS Origin (depending on the Misc. Integer settings, for the Generic Fanuc 5X Mill Post.) If you need to move the location of the WCS or Tool Plane Origin (this happens often in 5X Programming), then the Incremental depth options allow Mastercam to recalculate the correct positions, even though the Work Offset Origin is changing.

[Amsha]

18 hours ago, Colin Gilchrist said:

If you are defining Drill Points for a 5 Axis, I would highly recommend that you create a Point entity, at the actual top of your hole, and that you use Incremental for all your Clearance, Retract, Top of Stock, and Depth values.

Why?

Why would I recommend that you use all "Incremental" settings?

Because the depth values come from the "point" itself, relative to your Tool Plane and WCS Origin (depending on the Misc. Integer settings, for the Generic Fanuc 5X Mill Post.) If you need to move the location of the WCS or Tool Plane Origin (this happens often in 5X Programming), then the Incremental depth options allow Mastercam to recalculate the correct positions, even though the Work Offset Origin is changing.

You are correct, but i also work on 3 axis and sometimes i need to only get the posision of a hole and put the deep value on incremental, but mastecam dont do it, as you can see on post above. Why Mastercam is ignoring the Textbox of "Top of Stock" on calcs to deep, but using it for the aproximate value (...R2...)?

[Colin Gilchrist]

Mastercam is outputting 'R2' because that is what you put in the Retract box. The Retract parameter controls the R value.

[Amsha]

33 minutes ago, Colin Gilchrist said:

Mastercam is outputting 'R2' because that is what you put in the Retract box. The Retract parameter controls the R value.

if you look it, is on incremental too, if works for R value why didn´t work for deep, as i said the value in text box  " Top of Solid" only is used for R values and not for deep calcs, for deep calcs it´s use the Z Value of the entity. 

 

[Colin Gilchrist]

45 minutes ago, Amsha said:

if you look it, is on incremental too, if works for R value why didn´t work for deep, as i said the value in text box  " Top of Solid" only is used for R values and not for deep calcs, for deep calcs it´s use the Z Value of the entity. 

 

Huh?

Sorry, I'm really not sure how to interpret your response.

I know this; if Drilling in Mastercam was "broken", there would be a whole bunch of people complaining about it...

I don't mean that as an insult, but I don't personally see any difference between the versions.

Are you saying that if you use the exact same settings in X9 vs. 2018, that you get different output from the Post, using the exact same file? Try creating the same path in an X9 file and post the code. Then open the file in 2018, do a Save As with a new name, regenerate and Post the Op. If you are getting different output, I'd be happy to take a look. 

[vlan]

HI ALL

I could be missing something, but I think i have the same problem, with the contours,

Attached here is the program from MC2018, but if you post it with MC 2019, you will have the different result,

Mc 2019 ignores “top of stock” absolute and Incremental ??,

Can someone help me out, please,

Test.NC

TEST.mcam

Thanks

VN

[Guest]

2 minutes ago, vlan said:

HI ALL

I could be missing something, but I think i have the same problem, with the contours,

Attached here is the program from MC2018, but if you post it with MC 2019, you will have the different result,

Mc 2019 ignores “top of stock” absolute and Incremental ??,

Can someone help me out, please,

Test.NC

TEST.mcam

Thanks

VN

I would send it in to you reseller

[vlan]

after you open it with MC2019, regen tool path, then post it, you will see what i am talking about ...

Thanks JParis,

 i just wonder if i am missing something ..

 

[Guest]

4 minutes ago, vlan said:

 i just wonder if i am missing something ..

Your reseller can tell you....

It's an oddity and if there is a real issue, they will get it to QC