G90/G91 in canned cycles

[alfalfa]

Using Camsoft CNC Pro v15.8
I am trying to use G90 or G91 with G81. I am having problems and wondering if anyone out there has succeeded in doing so.

G54
G0 X-4 Y-1 X1
G90 G81 Z-1 R.15
X-3
G91 X-1
X-2
G90 X-20
G80

I want to maintain the drill cycle in Abs at all times, but at times want to move between holes in Inc then back to an Abs move. That being said, there may also be times when I want the drill cycle to be in Inc mode. (separate drill cycle)

I have played around with it for several days and feel like beating my head against the wall. Camsoft tech is helpful, but busy and several timezones away. Any other help would be great.

[camsoft]

Alfalfa,

Switching X,Y,Z to incremental could be done easily if you customize your drilling macro to trap for both modes. The X,Y abs/inc positions are going to be taken care of themselves but making a change within the canned cycle is going to affect the Z unless you customize the macro to keep track of Z.

You will find canned cycle drilling macros for both abs and inc G81 in the MACRO.MAC file of V15.8 but you would have to combine them to be able to switch modes while still in the cycle.

Most of us would advise you to pick one method or the other so an easier method would be to simply place a G81 on the G91 line to start a new canned cycle in incremental. This would be easier to do because you can add logic to call the macro of your choice when the drilling cycle starts rather than trying to trap for a mode switch or mixture. Just remember to add G90 after the end of the cycle or else the X,Y and Z's will continue to be incremental.

Tech Support
CamSoft Corp.
(951) 674-8100
support@camsoftcorp.com
www.cnccontrols.com

[Karl_T]

Just another note.

I see you don't have a feed rate in your G-code. The control will just sit there and appear hung up (feed is 0).

DAMHIKT (Don't ask me how I know this)

Karl

[alfalfa]

Right, it should include a Fcode, I forgot to add it. My main concern is switching between G90/G91. Also, on a slightly different topic, has anyone ever done a 5 axis mill using camsoft??

[Karl_T]

Camsoft:

I went looking throught the new default CBKs in 15.8 for one that uses the [G81 incremental] macro in macro.mac and also G98 and G99. Couldn't find anything. It would be real nice to inspect a CBK that can use drill cyles in either G90 or G91 <absolute incremental>modes and also in G98 or G99 modes<return to Z or R plane> There's four combinations here, and at least on first look, I don't see how to handle this.

IMHO, this should be included as standard stuff.

Karl

[alfalfa]

I would have to humbly agree with Karl.

[camsoft]

Check yourself for bites...

The drilling routines are right there in the Default.CBK and Macro.MAC files.

In the Default.CBK you will find these pre-written macros and G codes
[G81]
[G81 INCREMENTAL]

\998=1 ' return to initial point in canned cycle
-----G98
\998=0 ' return to Rapid plane in canned cycle
-----G99

The MACRO.MAC file has several alternatives plus each CBK made up for various machine types and models have there own variations.

[G73HighSpeed] 'G73 High Speed Deep Hole Drilling Cycle
[Bolt Hole Drill G181] ' Drilling of bolt patterns
[G83Standard] ' Description of G83 Deep Hole Drilling Cycle
[G83FeedDown] ' Description of G83 Deep Hole Drilling Cycle (Feed Down)
[G98 SET] ' Sets initial point in canned cycle
[G98 RETURN] ' Return method for G99 in G90 or G91 modes
Also the other canned cycles G82 through G89 are there as well.

We have been approached with over 40 varieties of drilling cycles over the years. We say to each his own, so we have been modulizing these canned cycles to call macros so each user can swap out the defaults with their own.

The provided drilling routines take care of the drilling cycles in G90 or G91 and also G98 or G99 modes but the original question posed to merge or mix the routines without ending the current cycle to start a new cycle has not been done. It can be done, but it would take some one to merge them together.

Tech Support
CamSoft Corp.
(951) 674-8100
support@camsoftcorp.com
www.cnccontrols.com

[camsoft]

Geof,

The power is in the knowledge that you can...

However, you're right we don't have it setup this way now. When asked in the past we just told people to begin another G81 but people tend to use cad/cam systems more these days that post in one format so when asking around here no one could even remember the last time we were asked. The X,Y take care of them self, so only Z would need to be kept track of if someone wanted to add it. There's a memo now suggesting this for the version.

Tech Support
CamSoft Corp.
(951) 674-8100
support@camsoftcorp.com
www.cnccontrols.com

[Karl_T]

I took a second look at default.cbk tonight. I'm 2000 miles from my control so I can only inspect logic. The code run during G81 is below.

My concern is with G98 <return to initial level> and G99 <return to R level>. It looks like if you call a G81 in G90 mode the drill cycle will always run in G99 mode. If you call a G81 in G91 mode the drill cycle will always run in G98 mode.Look at the last line of [[G81]], it commands a rapid to the R plane. And, look at the last line of the [[G81 INCREMENTAL]], it commands a rapid to the inital level.

Logic is needed in these two macros to check for G98 and G99. All the other drill macros need a similar modification. I see \998 is used for other purposes, I'd suggest a different variable.

Karl








Gcode.fil

IF \774=1 THEN GOTO :INCMODE
IF\775=0THEN\776=z:[G81]:\775=81:EXIT
IF\775=81THEN[G81]
IF\775=82THEN[G82]
IF\775=83THEN[G83]
IF\775=84THEN[G84]
IF\775=85THEN[G85]
IF\775=86THEN[G86]
IF\775=87THEN[G88]
IF\775=88THEN[G89]
EXIT
:INCMODE
IF\775=0THEN\776=z:[G81 INCREMENTAL]:\775=81:EXIT
IF\775=81THEN[G81 INCREMENTAL]
IF\775=82THEN[G82 INCREMENTAL]
IF\775=83THEN[G83 INCREMENTAL]
IF\775=84THEN[G84 INCREMENTAL]
IF\775=85THEN[G85 INCREMENTAL]
IF\775=86THEN[G86 INCREMENTAL]
IF\775=87THEN[G88 INCREMENTAL]
IF\775=88THEN[G89 INCREMENTAL]
-----G81


\998=1 ' return to inital point in canned cycle
-----G98
\998=0 ' return to Rapid plane in canned cycle
-----G99




macro.fil

[[G81]]
' G81
ISTHERE Z;\400;\401
IF\400>0THEN\776=\401
DECELSTOP
RAPID x;y;r
GO x;y;\776
DECELSTOP
RAPID x;y;r

[[G81 INCREMENTAL]]
' G81
' Call this routine from the GCODE.FIL file when in incremental mode
' R value for rapid clearance plane is incremental from the current Z position
x=0:y=0:z=0:r=0
ISTHERE X;\400;\401
IF\400>0THENx=\401
ISTHERE Y;\400;\401
IF\400>0THENy=\401
ISTHERE Z;\400;\401
IF\400>0THENz=\401:\776=\401
ISTHERE R;\400;\401
IF\400>0THENr=\401:\778=\401
DECELSTOP
RAPID x;y;0
DECELSTOP
RAPID 0;0;\778
GO 0;0;\776
DECELSTOP
RAPID 0;0;{0-(\776+\778)}

[Mr.Anderson]

You'll find good examples of G98,G99 and G83 in the Default.cbk file. This will show you how it was done in case you wanted to add it to any new canned cycles you or anyone else wrote but you can always do as I have. Place a [G98 Set] call as the first line in your canned cycle and a [G98 Return] call at the end just before EXIT. I saw you posted some camsoft internal logic but that may be copyrighted. I think you should just ask camsoft for these macros so you can make all your canned cycles this way.

[alfalfa]

Mr. A raises a good point that should be clarified as I know none of us want to be violating copyright laws. Camsoft - is it OK to post portions of internal code such as we have been doing in this thread? I believe that this is a great way to 1- have more than 1 or 2 minds working on something. 2 - get ideas for new upgrades (for Camsoft) 3 - pass on useful tips/solutions/workarounds for common or not so common issues that arise.

AL


De Oppresso Liber - Is 61:1-4

[camsoft]

alfalfa,

This is a touchy situation and for the most part we see that it really does help people. Speaking without the authority to say so, we would say legally speaking do not post CamSoft internal logic routines on a public forum. Some material is copyrighted by 3rd parties and much of it we ourselves should get written permission to publicly pass it along or hand out. Most people already have what they're looking for anyway. They just don't know where to find it and can view the logic for themselves if a poster wanted to point out to them as to where to find it. For people that can't find it they could ask us. We do have a full tech staff here.

On the other hand there are many very clever people out there. We are amazed sometimes at what has been done and can safely suggest that if you are the owner of the logic or wrote it your self then by all means post it. Much of what we add to our own files is that of our customers sharing these routines with us freely.

The benefits of what people have learned and shared with us over the years using CamSoft has snow balled into a vast library of routines spread over many computers here at our offices that even we can't keep track of what we have to offer sometimes.

This is your forum to discuss ideas with others. We are always listening to the discussions so we will step in and provide accurate information and also post routines or logic to straighten out any discussion that is mis-informing people. We honestly have seen much of this but we can't comment of every little thing. If you are serious and the answer is important to you please contact us directly. Depending on what you guys ask we can certainly post the logic legitimately.

Tech Support
CamSoft Corp.
(951) 674-8100
support@camsoftcorp.com
www.cnccontrols.com