Do you comment operations?

[Panda_Guy]

When I first started using Mastercam, the company I work for had just hired another programmer who had been using it for years.  Our manager wanted us to standardize our methods so what was hitting the shop floor was consistent regardless of who programmed it.  One of my requests  was comments on every tool and every operation.  The other guy said, "That seems like a lot of typing.  If the set up guys want comments, they can add them."  I couldn't believe he was serious, but that was how he was used to working.  His programs were basically a black box and if anybody needed a simple tweak, they had to go to him for it.  I feel a lot better if the guy executing the code is aware of what I am trying to do.  

[Newbeeee™]

THE big thing about all of this, is as a programmer, your job is to make the set-up guys job as easy as possible.

If you're not doing that, you're not doing your job right imo. As much clear and concise info he needs, you must supply.

If the spindle isn't turning, then you aren't earning

[jeff]

I have mine set up where I comment on EVERY operation. rough pocket, finish, drill, etc....

And my post spits out N numbers ONLY at those comments so my programmers can easily start at any op they want.

G15's (or G56 for you Fanuc peeps), S,F and tool height are output at every op.

[MIL-TFP-41]

on every operation...no. Every toolchange and any plane change, yes. Usually simple things...like "rough face front" or "tap holes left side" get the message across.

I am stealing Bob's idea with writing to a macro value the operation number.

[jlw™]

Thanks for the idea Bob, I implemented it this morning.

 

Ron, I have postability post so it was easy for me.

 

I planned to add it to the pn line but it came up about 8004 times so i added it to my pcomment3 section like this:

 

Here is the result:

 

Thanks again for the idea Bob!

[Bob W.]

fmt  "#750=" 2 op_number         #WDS 6/27/2015

psof
      op_number = opnum, e$   #WDS  6/27/2015
      pbld, n$, op_number, e$     #WDS   6/27/2015

Here are the changes I made to my post.  I also added it to the ptlchg0 (null tool change) and ptlchg (tool change) sections.

[Bob W.]

Also, I don't label my programs but I probably should.  I gave my operators a seat of Mastercam on a shop floor computer (computer cart) so if they have questions they can open up the program and follow along.  There are to be no edits allowed on the floor however, all edits go through the office.

[Sticky]

Nice idea Bob, I'll be stealing that one!

[Bob W.]

Glad I could help and finally make a contribution.  Another tweak I made to my horizontal posts recently was the addition of a work offset wipe macro call (G65 P9970).  All of the programs that run on my horizontals have the offsets set in the program header.  Before the offset is set I wipe all offsets and set them to zero.  I also do it at the end of the program so if for some unexplained reason the manual entry doesn't get entered in Mastercam the machine will generate an over travel alarm because it will be trying to machine at the machine origin (X0,Y0,Z0).  I try to set things up so it would take several screw ups on the same project to result in a crash.  Can't have enough layers of safety and it doesn't take any extra effort or time once it is in place.

[Sticky]

Why use a mnp for offsets? If you have them in your post they should be pretty robust. I've been doing it that way in MC for a while and it has been bomb proof.

 

Doing an offset wipe isn't a bad idea though.

[Bob W.]

Why use a mnp for offsets? If you have them in your post they should be pretty robust. I've been doing it that way in MC for a while and it has been bomb proof.

 

Doing an offset wipe isn't a bad idea though.

I use manual entry because not all of the offsets are in the same location.  We use DFO and not COR so with each new program we establish the offset location based on CAD data and standard offset location tables based on the fixture, etc...  Once it is set it never gets tweaked, it is good to go.  Is there a better way?

[buck30]

I Always leave some sort of comment, simple may it be.

But Where I Have run inot trouble is bracket inside another bracket   eg.  ( tool 3 (regrind)  small pocket)

This makes my Robo drill fault and give me an error message.   Easy to fix but it dosn't make sence to me since the machine dosn'r see anything inside ( ......)    

Little thing i have learned not to do but reading this thread made me wonder again????

[BenK]

I Always leave some sort of comment, simple may it be.

But Where I Have run inot trouble is bracket inside another bracket   eg.  ( tool 3 (regrind)  small pocket)

This makes my Robo drill fault and give me an error message.   Easy to fix but it dosn't make sence to me since the machine dosn'r see anything inside ( ......)    

Little thing i have learned not to do but reading this thread made me wonder again????

 

I have ran into this before. The control reads the close bracket and thinks the comment is finished. Than it sees anything after that as code. A better practice would be to wright the comment as follows. 

 

( tool 3 - regrind - small pocket)

[Mgrenier]

The way around the bracket for us was to use the square brackets "[ ]"  that are used for Macro B on Fanuc.

 

It's just a matter of getting used to write it that way. It will look like this: ( tool 3 [regrind]  small pocket)

[Newbeeee™]

Glad I could help and finally make a contribution. 

LOL!

Trust me Bob, you make a big contribution here.

[crazy^millman]

Thanks for the idea Bob, I implemented it this morning.

 

Ron, I have postability post so it was easy for me.

 

I planned to add it to the pn line but it came up about 8004 times so i added it to my pcomment3 section like this:

 

Here is the result:

 

Thanks again for the idea Bob!

 

Thanks yes with Postability you have a lot of the leg work done. Might be a good suggestion for Dave to add a switch for this in his posts.

[crazy^millman]

fmt  "#750=" 2 op_number         #WDS 6/27/2015

psof
      op_number = opnum, e$   #WDS  6/27/2015
      pbld, n$, op_number, e$     #WDS   6/27/2015

Here are the changes I made to my post.  I also added it to the ptlchg0 (null tool change) and ptlchg (tool change) sections.

 

 

Thanks Bob and great suggestion. I can see this being something we implement Company wide for all of our customers move forward. Being offsite every thing we can use to help us track down any possible problem will be a huge time saver for us and our customers.

[Sticky]

I use manual entry because not all of the offsets are in the same location.  We use DFO and not COR so with each new program we establish the offset location based on CAD data and standard offset location tables based on the fixture, etc...  Once it is set it never gets tweaked, it is good to go.  Is there a better way?

 

I don't use COR either, but I don't use DFO.

 

My post has my cor stored in it. When I program, I am programming an assembly of the pallet, and all fixtures on top of it, plus the parts. Each T plane has it's own offset, these are set off the needs and requirements of the parts. My post calculates the position of each tplane and offset against my cor, and then outputs the correct machine coordinate in the header of my program.

 

Once I got it work it's been completely reliable. The only time I ever need to pick up an offset on the machine now is when I am doing a quick repair part or the like and I am programming on the control. Otherwise I can take any new customer part, throw it on any of 27 different pallets or tombstones inside of mcfsw, and have anywhere between 1-200 offsets calculated for me without having to go to the machine and everything will be spot on.

[buck30]

Thanks guys all good ideas.      

But the biggie from all this is YES fill out some sort of note on every operation.

I find it really comes in handy when you start moving the order of operations around.

[jeff]

Also, I don't label my programs but I probably should. 

 

Your operators will thank you if you do.  

And it also cuts down on the questions they have. 

[BBprecise]

If the tool is only doing 1 or 2 features before the next tool is called I don't put comments on the tool (I'll put them on our s/u sheets as it's just a few lines). If a tool is doing several features I will put what feature it's cutting into the prg. when it gets to that feature. This mostly applies to our mills and horizontal turning centers. On our VTL's, we cut with ceramics mostly and it make take several passes to rough that feature so when the tool goes to a position so the operator can index the insert (or measure the part if needed) at the next beginning of the next pass I'll put "1st pass to rough yadayada", "2nd pass to rough yadayada" and so on. That way the operator knows exactly which roughing pass he was on and which one is next if he has to jump out of the prg. for some reason. At every M0 in a program (for whatever the reason for the M0) we always put what we call a safe start block. Basically it's just the information you find at the beginning of a lathe tool (tool number, offset, SFM, spindle direction, G96/G97) and we also put the tool change command (some of our VTL's require the M6 others that are turret style do not require it but the prg. has it anyway and the machine just skips it). We do not allow operators to start in the middle of a toolpath unless given permission from the supervisor and the supervisor has to be standing there when doing so. If the operator has to jump out of the program to re-run a previous toolpath they are required to run rapid override at 25% in case they called up the wrong toolpath. On our lathes the only lines that get numbered are the tool change lines, and the controls display that line number which helps get the operator back to the right spot. We've had people jump out of a program, call up the toolpath that was for another tool and since there wasn't an M6 to call up the correct tool they crashed the machine. This was before we implemented forcing a toolchange command on every toolpath. We call it idiot proffing and saving our bacon with customers. Customers don't like it when you tell them you just plowed into the part which means they have to forge another part because the grain was altered because of the impact.

[Thee Rickster ™]

I always write in the comments this:  Your turn turn buy coffee!

[gcode]

I write comments in the operations as much for me as for the operators

I don't know how many times I've been filling in a comment... to discover there was a problem with the OP

 

The comments are also very useful when you're making edits to a 3 or 4 year old file..

[Bob W.]

I guess one of the main reasons I don't write comments is due to how our processes are set up.  The operator's main responsibilities is verifying that the correct tool is loaded in the spindle and performing first article inspections.  We Vericut everything so the program is good and the operator typically watches the first move to make sure the offset is set correctly, then hits option stop and walks away.  When the next tool comes along the operator verifies the tool, then starts the machine and walks away to do something else.  One of my operators just about crapped when a tool was approaching the work piece at 5% rapid and I walked up and set the rapid to 100%.  I knew the tool was good and I told him we paid $xx,xxx for Vericut and that is one of the ways we get a return on the investment...  The only ways we will crash a machine is if the tool is set up incorrectly, wrong setup, or the offset is not correct.  Two of those are ruled out on the first move of the first tool of the program.

[Newbeeee™]

 One of my operators just about crapped when a tool was approaching the work piece at 5% rapid and I walked up and set the rapid to 100%.  I knew the tool was good and I told him we paid $xx,xxx for Vericut and that is one of the ways we get a return on the investment...  The only ways we will crash a machine is if the tool is set up incorrectly, wrong setup, or the offset is not correct.  Two of those are ruled out on the first move of the first tool of the program.

Hahaha - Bob, you got bigger Cahoonas than me

I'd always slowly let the tool come to the feedplane okay to check the tool offset before letting it go.