Syil X3 Drilling Problem

[wwendorf]

Hi all,

I've been having a weird little problem with Dolphin v9 (soon to be v10) and my Syil X3.

When I do a drilling cycle, I choose peck drilling and a clearplane of .25 and a traverse plane of 1".

Instead, when my X3 goes to drill those holes, it does a deep drill (ie. down to -.1, up to .25, down to -.2, up to point .25, etc...) instead of my understanding of a peck drill (down a bit, up a bit, down a bit more, up a bit, etc...). In addition, instead of going up to the +1" mark before it moves to the next drilling location, it travels at .25 (my speed change plane).

Anyone got any ideas? I'm using the M_Mach3.ppr post as I got it with the v9.

I've managed to accommodate the problem in my programming, but it still bugs me a bit.

Rodney suggested I post the question on here and that perhaps John S. could give me a hand.

Thanks,
Wade

[John S.]

Wade,
It's the crappy M_Mach3 post.
That post was sent to Dolphin by a user who modified it to suit the way he worked instead of industry standard.

I have run a file of mine thru that M_Mach3.ppr post

Run at clear plane [ box ticked ]
Peck drill 4 pecks
N12 G99 G83 X70.0 Y0.0 Z-7.833 Q1.958 R3.0 F90

Run at feed plane [ no tick ]
Peck drill 4 pecks
N12 G98 G83 X70.0 Y0.0 Z-7.833 Q1.958 R3.0 F90

Run at clear plane [ box ticked ]
Deep drill 4 pecks
N12 G99 G83 X70.0 Y0.0 Z-7.833 Q1.958 R3.0 F90

Run at feed plane [ no tick ]
Deep drill 4 pecks
N12 G98 G83 X70.0 Y0.0 Z-7.833 Q1.958 R3.0 F90

Note that if the traverse box is ticked it should travel at clear plane but G99 is feed plane, the G98 and G99's have been swapped.
Also note that no matter what cycle type is selected it uses G83 all the way thru.



Now using a decent post

Run at clear plane [ box ticked ]
Peck drill 4 pecks
N 110 G98 G73 X70. Z-7.833 Q1.958 R3.0 F90.0

Run at feed plane [ no tick ]
Peck drill 4 pecks
N 110 G99 G73 X70. Z-7.833 Q1.958 R3.0 F90.0

Run at clear plane [ box ticked ]
Deep drill 4 pecks
N 110 G98 G83 X70. Z-7.833 Q1.958 R3.0 F90.0

Note with this post that G98 and G99 are the right way round.
Also note it uses G73 [ high speed peck ] for the peck cycle.

Try this post and see how you get on.

[wwendorf]

Thanks John!

I'll be giving this a try tonight when I get home.

I'll report back how everything works.

Thanks again!
Wade

[wwendorf]

Well, I finally got the chance to try your new post and it didn't work for me. Using the Mach_3.ppr I got a GCode file that was 485 lines long. Using the one you posted here, it was over 7700 lines long?!?!

I attached them in zip files, along with the .cnc file.

Thanks,
Wade

[wwendorf]

One question, I just upgraded from Partmaster 9 to Partmaster 10. Would that post you created still work properly in v10 or was it strictly for v9?

Wade

[John S.]

No it should still work.

I'm looking at the files you sent, the increase is partly because yours is in ones as regards numbering and mine is in 10's and it also puts the z on a separate line.

Much of the code length is due to ramping down into the circles and I must admit I hardly use ramping.

Can you explain some of the operations as I can't follow them.
In operation 4 you have it offsetting left at 0.5" deep
In operation 5 you have no offset but the same tool and cutting 0.425" deep
In operation 6 Again you have no offset, your Z is -0.400" and depth of cut is 0.-25" deep which is the same as operation 5 ??

Operations 7 and 8 seem to be doing the same thing as regards depths.

Operation 9 seems to be selecting the same tool as Operation 3
Ignore that just spotted the feed rate change.
You can do this by clicking on the big blue F in the icon box at any point instead of editing a tool profile BTW.

You are removing the centre portion to a depth of 0.500" and the phase hub recess to a depth of 0.425" but by using a goround and not area clear or pocket do you realise there is a ring left unmachined just outside the centre hole.

.

[John S.]

Ooops forgot to add.
Here's the standard M_MACH3 post with the G98 /99 changed over and G73 high speed peck added.
The ppx and ppr are both zipped here and I have added an underscore at the end so it doesn't overwrite the original one.

[wwendorf]

Originally Posted by John S. No it should still work. Can you explain some of the operations as I can't follow them. In operation 4 you have it offsetting left at 0.5" deep In operation 5 you have no offset but the same tool and cutting 0.425" deep In operation 6 Again you have no offset, your Z is -0.400" and depth of cut is 0.-25" deep which is the same as operation 5 ?? Operations 7 and 8 seem to be doing the same thing as regards depths. Operation 9 seems to be selecting the same tool as Operation 3 Ignore that just spotted the feed rate change. You can do this by clicking on the big blue F in the icon box at any point instead of editing a tool profile BTW. You are removing the centre portion to a depth of 0.500" and the phase hub recess to a depth of 0.425" but by using a goround and not area clear or pocket do you realise there is a ring left unmachined just outside the centre hole. .

Operation 4 - Cuts the inside of a hole down all the way thru my material.
Operation 5 - Cuts directly on the line to a depth of .425 using ramping.
Operation 6 - As ramping doesn't level off until you finish the cut, there is a part of the material that is higher. This operation goes down to the depth of .45" and levels off the ramping that is left.
Operation 7 - Does a ramping cut on the inside of the PhaseHubRecess.
Operation 8 - Does the same as #6 except on the PhaseHubRecess.
Operation 9 - Thanks for the tip on the feed change. Didn't know about that one.
Operation 10 - Cleans up the inside edge of the CenterHole

Actually, because I cut using Operation #5 where it cuts directly on the line that makes up the CenterHole, that takes away any issue I have of a ring of material being left over.

I tend to use this method for removing material in certain instances because I get very fast removal rates using ramping. I also get really good results with it.

Thanks for all your help.

I will try the modified post today.

I did try the first post you put up, but I had nothing but problems getting my machine to operate it. I use tool offsets and mach3 was totally wiggin' out while trying to perform operations on the mill.

Wade

[wwendorf]

Originally Posted by John S. Ooops forgot to add. Here's the standard M_MACH3 post with the G98 /99 changed over and G73 high speed peck added. The ppx and ppr are both zipped here and I have added an underscore at the end so it doesn't overwrite the original one.

Hi John,

Been a long time since we chatted on this thread. Anyway, i've run into another problem with what I believe is the post processor again. I am trying to use my 4th axis, but it won't engage. I'm trying to make dolphin treat A as Y which will work for my needs, but when I postprocess, A never gets added in.

Can you help me?

Wade

[HJozsi]

Originally Posted by wwendorf Hi John, Been a long time since we chatted on this thread. Anyway, i've run into another problem with what I believe is the post processor again. I am trying to use my 4th axis, but it won't engage. I'm trying to make dolphin treat A as Y which will work for my needs, but when I postprocess, A never gets added in. Can you help me? Wade

Hi Wade,

just download and try the 'M_MACH3R.ppr' from ***********

http://tech.groups.yahoo.com/group/d...20Files/Mach3/

it is a Mach3 post processor with Rotary A & B axis support ...

Good luck

Jozsef

[wwendorf]

Awesome! Thanks!

I'll try it tonight!!!!

Wade

[HJozsi]

You are welcome ...

And I wonder about the result then ...

Actually I've a friend, who has a new Siyl X3 also with rotary axis...
we plan to try the rot axis soon ...

Here it is one of the first machining video with PartMaster and X3

http://www.cnctar.hunbay.com/HJozsi/..._Mach3%202.wmv

Jozsef