Help!!!! Drill Cycle

[tsaladyga]

Hi Guys,


I have a situation. I am new to Pro Manufacturing. When I program a drill cycle, after the G80 command I get a G0 Z0 line that I have no idea where it is coming from. Anybody know how to get rid of this line? All suggestions much appreciated.The code looks like this...


T4 M6
G0 G54 X4.0054 Y-2.5669 M3 S3055
G43 Z2.5 H4 M8
G81 G98 X4.0054 Y-2.5669 Z-.1 R0.25 F4.5
X0 Y-4.8794
X-4.0054 Y-2.5669
Y2.0581
X-1.197 Y4.213
X0 Y4.2456
X4.0054 Y2.0581
G80 Z2.5
G0 Z0
M9
G0 G49 Z0
M1

 

[Mr Ray]

Could it not be the retract plane?

 

[tsaladyga]

It could be. I am pretty sure the problem is in the set-up of the OP10 or the Machine set-up. I am just not sure what I am doing wrong. When it asks for machine zero, is that the datum point of the part? Or should I be making a datum point where machine home would be?

 

[Mr Ray]

Part Zero should in relation to the part. Then create a clearance plane based on this location. Right click on the sequence <Edit Definition< Put a check mark in Seq Setup> Put a check mark in Retract surf> No w enter a value for a clearance plane and see if that Z value changes after you run the tool path.

 

[tsaladyga]

I am getting the settings all wrong I think. I can't get this thing to spit out what I want it to do. I keep getting extra "Z" moves at the beginning or end. So frustrating.


T4 M6
G0 G54 X4.0054 Y-2.5669 M3 S3055
G43 Z2.5 H4 M8
G0 Z0.25 <---------now I get this(this line shouldn't even be there)
G81 G98 X4.0054 Y-2.5669 Z-0.1 R0.25 F4.5
X0 Y-4.8794
X-4.0054 Y-2.5669
Y2.0581
X-1.197 Y4.213
X0 Y4.2456
X4.0054 Y2.0581
G80 <-----this is supposed to be G80 Z2.5
M9
G0 G49 Z0
M1

 

[Mr Ray]

I hear ya on getting frustrated!


Is the clearance (retract) value .25? If not then perhaps your CHK_SURF_STOCK_ALLOW is .25. You must have a .25 hid in there somewhere....

 

[TonyJager]

In you first example you posted it looked pretty good. You were just concerned about you z after the G80.

Couple of things.

At your oerations/machine setup setup pick your from point and home point. For my setup it is usually the machine home.
Also check in the workcell setup and check cl command output options. Mine is usually set to only at start.

As far as the retract at the nc level it is usually relative from your part/csys or a plane above the part.

Also make sure you picked the sequence_csys in the coordinate_output.
Couple of parameters to look out for: clear_dist (normaly I set it to .05) so the drilling will start .05 from where the hole starts.
pullout_dist I set to 0
and rapto_dist to 0.

This should give you what you want. I not, there may be some option in the post you can tweak.

Hope this helps.

 

[tsaladyga]

Thanks Guys!!!


All the suggestions helped alot! It sucks when you're new to this and there is noone to help give advice. I appreciate it.











Todd

 

[Guest]

In your first example it looks like you are using a PULLOUT_DIST of 2.5 which activates G98 in the post. When using PULLOUT_DIST you must set your retract plane to 2.5. This should give you what you want.

 

[cncwhiz]

Hi Guys,


I have a situation. I am new to Pro Manufacturing. When I program a drill cycle, after the G80 command I get a G0 Z0 line that I have no idea where it is coming from. Anybody know how to get rid of this line? All suggestions much appreciated.The code looks like this...


T4 M6
G0 G54 X4.0054 Y-2.5669 M3 S3055
G43 Z2.5 H4 M8
G81 G98 X4.0054 Y-2.5669 Z-.1 R0.25 F4.5
X0 Y-4.8794
X-4.0054 Y-2.5669
Y2.0581
X-1.197 Y4.213
X0 Y4.2456
X4.0054 Y2.0581
G80 Z2.5
G0 Z0
M9
G0 G49 Z0
M1

I see a few problems with your g code. First off I think that you are going to have a big problem with the "G49" at the end of the program. You did nit tell us what the control is, but most fanuc controls newer than the 6M won't like it and will rapid to "Z0" before returning home. Your first post looks better than what you posted out after. You don't need pullout of any other parameters for a standard drill cycle. You post processor needs some tweeking to resolve all of your issues. You look like you are using a post processor that came with the software. We can be of more help if you post details "control type and model, machine etc...".

 

[tsaladyga]

cncwhiz


SorryI missed on the G53 in the same line. Actually it does work. I use it on a Haas VF-5. I actually have used that format for about 15 years now and never had a problem. I am an experienced programmer, just new to Pro Manufacturing(I was an avid Mastercam user for the last 10 + years) Where I work now mandated that we have to use Wildfire 4.0. No one here knows how to use it so I am the guinea pig!It is a very complicated system. Not saying it is garbage at all, just alot more muddled than Mastercam. I figure I have a lot of learning to do and it is hard when you don't have any support. I am using Posthaste for my post program. I like it alot better than G-Post. Just my opinion. Anyways, I figured out the problem with the help from the guys above. But I appreciate all the help I can get! I included the right format below.


T4 M6
G0 G54 X4.0054 Y-2.5669 M3 S3055
G43 Z2.5 H4 M8
G81 G98 X4.0054 Y-2.5669 Z-.1 R0.25 F4.5
X0 Y-4.8794
X-4.0054 Y-2.5669
Y2.0581
X-1.197 Y4.213
X0 Y4.2456
X4.0054 Y2.0581
G80 Z2.5
G0 Z0
M9
G0 G49 G53 Z0 <-----this is the way it correctly outputs
G0 G53 X0 Y0
M30
Edited by: tsaladyga