Rapid to linear in operation...

[William Grizwald]

Is there a setting to change the default rapid of A SINGLE OPERATION to a linear feed? The purpose is for preventing dogleg moves for that op only. The operation in question is a drilling op.

 

TIA.

 

--

Bill

 

MCX 2

[crazy^millman]

Could you use the G85 cycle to do the same task for drilling? You could do this with a Mi and get the posted code to output a certain operation as G1. Will take a little bit of work. Look at every where there is posted code and put in something like this before sgcode.

 

[if mi5 = 1, gcode$ = 1] I think this will make that operation output only G1 instead of G0.

 

Again backup your post before trying anything.

 

HTH

[William Grizwald]

I was hoping for the simple "Rapid Feedrate" field in the operation. I'll just retract all the way out as a work around.

 

--

Bill

[Guest]

I don't understand why something that is very out of the norm is a "workaround"?

 

 

With that being said,

You could also if you wanted to spend the time use a point move and then edit it to get a feed rate move to the next position.

[William Grizwald]

"I don't understand why something that is very out of the norm is a "workaround"?"

 

Perhaps to some, very out of the norm... For me it's drilling a series of holes down in a long diagonal slot. The slot is 1" deep and the hole spacing is such that the dogleg would send to tool into the sides on rapid if I keep the R plane close. That said, I came from a system that had a simple field to set a feedrate for rapids within each operation. It allows one to use a fast G1 for true point to point just on that operation. Just something I was used to...

 

--

Bill

[Ron Branch @ Verisurf]

Well what I doing was giving you the same thing. You can get facny and have it defualt to your post's highfeed rate for retracts. Just depends on if you want to bitch about Mastercam or change somethings to get what you want.

[William Grizwald]

Ron,

 

Thank you very much.

 

Regards,

 

--

Bill

[Rick Henrickson 65]

Just curious, cant you just rapid to within .1 in z feed down rapid up to . 1, rapid to clearance rapid to next position rapid back down to .1

swithcing between your G98 and G99

or does this take longer then the feed option?

[William Grizwald]

Rick,

 

Yes, that is what I'm doing now. I retract using G99. It works ok. In the end we go through our programs tool by tool and operation by operation to sqeeze out waste. Our parts large, long term production on large machines, hence anytime we can reduce the air moves the better.

 

Btw, I passed this on the QC as an enhancement. Other systems have it, we should too.

 

--

Bill

[Roger Peterson]

Just curious, how do you get a canned drill cycle to feed between locations? Or are you outputing code longhand?

 

I too would like this feature. I use the toolpath editor to change a rapid to linear, and have setup posts to do this on an entire toolpath basis. We have this ability in the highspeed toolpaths. How much "most" people would use it unclear, but probably not much. I just don't know how you can make a canned cycle linear move between holes.

 

FYI, you can edit jump heights between individual holes via change at point if that helps you.

 

Thank you,

[Rick Henrickson 65]

Hey William another question how come the machine dog legs? is there maybe a parameter to fix this so the machine will move point to point instead of dogleging?

[William Grizwald]

Roger,

 

I'm retracting above the slot to clear then moving. The G99 insures a rapid back to the engage point. I'm not currently feeding between holes. The scenario would be a field for "rapid feed rate". By entering a value other than 0, the post would then output a G80 and fresh G8x for every hole thereby allowing a G1 between holes. It would be seamless to the programmer.

 

Rick,

"Some" machines here could be set for no "dog legs". The issue is to keep the MCX file generic enough that the program can be easily reposted for different machines. We're trying to standardize the process for most programming issues (and it's killing me... ).

 

--

Bill

[crazy^millman]

William how about you send me your post and let me add this to your post if you are not opposed to using mi vaules for an operation when posting.

 

Just to explain myself I perosnally would rather see CNC put resources to MATTS then a feature like this. Again I have been doing this for 20 years and problay needed to do this maybe 3 times in that amount of time. The ability to modify a post and get Mastercam to output your code the way you want is what makes it great.

 

How much do you really need this?

[William Grizwald]

Ron,

 

Thanks for the help. Yes, we use misc values (I think that's what you meant by mi?)We put our work offset and W axis positions there now (special TC macro...). It's not a deal breaker to not have a field in the operation. I'll play with the post later during lunch. The only down side is some users here "forget" about that area when copy/pasting ops. I'm sure you agree, when there are a 100+ ops and folks need to do quick changes... It pays to be a simple as possible.

 

--

Bill

[crazy^millman]

Well again with X changes to Mi(misc vaules) is very easy and then you are done even for 100+ operation.

 

I have a Mi for retracts that one machine does not need and use the same post for a machine that does need them. Yes I could several different posts, but I just turn on and turn off the mi post and done with it. Most times I put 2 or 3 machines in a file that is postes to different machines and just copy operations to all 3 giving me the ability to post to all 3 from one post but have it do 3 different things. The beatuy of X.

 

HTH