Subprograms thru Transform Translate Question?

[Kenneth Potter]

I have a bunch of holes to drill(32) thru double walls .Each hole location is NOT ! an equal distance from the next location (staggered)

 

i creates some vertical lines to get my rapid to, feed thru (top wall) ,Then rapid to,& feed thru (bottom wall).Then rapid completely out. Then use the 3D contour path & chain at point to insert my rapids & feed at my selected points.

 

Next I used Tranform Translate & with Subprogram turned on & find that all the translate options are only equal distances polar, rectanglar between points, ect:confused:

 

So i ask this question. How can I Dynamically select Multiple Staggered locations to Subprogram?

 

Thanks

 

Kenneth Potter

I got a Mastercam looove Jones

[Travis_Buchanan]

Are the holes different depths? If so how many different depths? All at different depths? You say staggered, do you mean non uniform grid and/or non polar coordinates?

--

Buzz Lightyear

[Kenneth Potter]

The depths are all the same.& all on the same plane . Its the locations.There are NOT an equal distance from each other .There all staggered from each other.

 

X1.0 Y0

X2.5 Y0

X4. Y.25

X4.75 Y-.25

X6. Y.5

X8 Y-.5

(ect)

 

What to do What to do !

 

I can program each hole the long way but it makes for a huge file on a controller that sucks for memory.

 

Thanks

Kenneth Potter

[Travis_Buchanan]

I'm not experienced with using cycles in Mastercam. I do however use sub-routines & cycles all the time. I would do a simple drill - no peck on all the holes then after posting code do a search and replace and manually edit the code. There is a way to do this in mastercam using "misc cycles?" I think. Our dealer set us up a bunch of preprogramed mortise cycles to select from simple drill - no peck, but I never use them. Here is an example of how I would do it after posting code. Fanuc code.

 

O0099( POSITION & SUB )

G00 X2.5000 Y1.0000 Z1.0000

M98 P0005

G00 X3.0000 Y0.5000 Z1.0000

M98 P0005

.

.

.

M99

 

O0005( DRILLING SUB )

G00 Z.1 <---- RAPID TO ABOVE FIRST HOLE

G01 Z-0.5000 F10. <---- FEED THRU FIRST WALL

G00 Z-1. <----- RAPID TO NEXT WALL

G01 Z-1.5 < ----- FEED THRU NEXT WALL

G00 Z1. <--- RAPID OUT OF PART.

M99

 

--

Buzz

[Kenneth Potter]

Well fo now i will translate the subprograms between steps & hand edit the right locations in.

 

Custom drill cycles is to much of a bother for me at this time. Iv been playing around with this translate subgrams for sometime & getting real frustrated at not being able to select all the Non- uniform point locations to sub out from the source operation. I keep thinking there a way to do it. And or if it can be done.

 

I,ll keep trying though.

[Kenneth Potter]

On my transform translate parameter page there a section thats totally greayed out

Its labled "Group NCI output by" with three selection options #Operation #Unique subprogram &

#Operation type. I cant for the life of me get it active. Is everyone elses Greyed out ? Mastercam L3 *8.1 .

 

I think this is why i cant select my subprograms NON uniformed location points ?

Help Help

 

Kenneth Potter

[cadcam]

Ken are you talking about this:

Group Nci

[Kenneth Potter]

Yup thats it cadcam . It stays greyed out no matter what i try to do. Maybe a reinstall & a complete up to date patch will do???

[cadcam]

Try going back in to the window and clicking on rtatit then back to translate and see if it comes alive.

[Glenn Bouman]

If you are only selecting one operation it will be greyed out. That function is non-applicable for 1 operation.

If it is still greyed out after selecting 2 operations toggle the Toolplane/coordinate option under Method.

[Kenneth Potter]

Glen Sir

That did the trick. I now know that for the Group NCI by option I must select two of more operations. The help balloons for each option explains there function . The just for different operation grouping methods

 

But it still gets me back to my original dilema. How can i select mutipul non-unformed (staggard) point locations to subprogram

 

Kenneth Potter

 

[ 02-04-2002, 06:57 AM: Message edited by: Kenneth Potter ]

[Allan Brown]

Can't do it as far as I know, but would make a wicked enhancement. You are looking for a point select menu (like in drilling) to pick a non-uniform translation pattern - correct?

 

I like Buzz's drilling sub method to call out the positioning moves followed by a sub call. I actually have added a "Subprogram Call" drilling cycle to all posts used by one of our customers. The only parameter is the sub number to call out.

 

[ 02-04-2002, 04:36 PM: Message edited by: Dave Thomson ]

[Kenneth Potter]

Yes Dave thats what The H----i,m looking for "POINT SELECT MENU". I thought it was already there & somehow was missing it! If one can do it in the drilling ops subout why not in the transform translate subout ???

Another thing i notice about Mastercams subprogramming is that theres no or little control over the subprogram numbering. The system preselects the subprogram number! M98P001, M98P0002, M98P003 What a drag! This is really really a bumming drag! Most subprogram numbers Kinda reflect the Main program numbering. Thats usually one or two intergers larger or smaller from Main program numbers.

If one can select the main program number/lable by way of common toolpath parameter settings of your choice ,WHY not the subprogram number?

 

I played with this for hours Just to find out that I still have to hand edit a ton of stuff.Oh well Live & learn(sad).

 

Dave I agree this would be a wicked powerful enhancement & in my opinion shoulda been there in the first place. Can you inform CNC software of this? Maybe it can added to V9 Before its released?????????

 

Kenneth Potter

[cadcam]

quote:

---

Maybe it can added to V9 Before its released?????????

---

Ken, to late.

 

[ 02-04-2002, 09:39 PM: Message edited by: cadcam ]

[Travis_Buchanan]

Thanks. I do some weird stuff in programming according to anyone outside my factory. I use sub routines all the time and each of my programs usually consist of 6 to 30 sub programs. I do this for neatness of programming and it is a standard way of writing programs "for us" that I developed years ago. It has made a big difference in the day to day programming & set-up of our machines. For example the set-up people know that O0099 is always the main loop, and the first thing in there is all there tooling and set-up infromation. It also contains all the saftey stuff like spindles off & retract, return all axis to 0. O0099 calls sub O0098 and sets it in a repetitive loop. O0098 is what I call the tooling control loop. It loads the tools, selects the tool offsets, work offsets, set the spindle speed and direction, etc, then calls the sub routine for that tool. This keeps the G code all seperate from the M code. I know it don't make any difference to the machine but it does to me. I may also call a sub routine from a sub routine such as a custom drill cycle or for any repetitive task. I just did a part that had 86 elipses that had to be machined with 4 different tools. I drew a circle at the center of each one and posted a simple drill program first. Then I did an incremental post on one of the ovals. For the final program it positions absolute and calls an incremental cycle. I did not have enough memory to write a total absolute program anyway, and this is a simple way of doing it.

--

Buzz

[Kenneth Potter]

To late! Darn!

 

Well how about a V9.1 or a 9.1.1 fix. Cant see waiting untill V10. What about a Chook Enhancment & putting it up for sale?

Just starting to get real deep in to subs & nested subs as a powerful tool.And i really hate the current limitation we now have.

 

Hey Buzz i like your way doing subs . Really keep thing neat & organized. So im gonna follow your lead & do the same.

 

Kenneth Potter

[Allan Brown]

quote:

---

Most subprogram numbers Kinda reflect the Main program numbering. Thats usually one or two intergers larger or smaller from Main program numbers.

---

The latest version of Mpmaster uses subprogram numbers that are incremental from the main program number. Mastercam uses 0001+ and 1001+ numbering based on the style of sub (translational vs. depth cuts, etc.). Mpmaster now uses [main progno] + [sub increment] and [main progno] + 1000 + [sub increment] numbering.

 

I also just added in the Subprogram Call drilling op. You still need to generate the sub properly on your own.

 

[ 02-05-2002, 01:14 PM: Message edited by: Dave Thomson ]