What's new
What's new

Stuck!

Scoop

Plastic
Joined
Jun 30, 2020
Hi guys,

Would appreciate your help with something as I haven't been machining very long, so my experience if not as great as most of you on here.

I have completed a job previously (a batch of parts) have a proven program on a VF4 Haas that uses 4Axis. I have been asked to leave on 10 thou / 0.25mm to each side of this part (so part will sit higher on the fixture plate) to allow for skimming / any errors. The part is therefore sitting 0.25mm higher on the plate, and the very top face of the part is therefore 0.5mm higher than intended. The program has essentially been written long hand as no CAD/CAM.

How do you think it's best to adjust the heights? I cannot simply put a 0.25mm tool offset in because some tools are used in multiple A axis angles.

Any ideas for resolving this would be greatly appreciated.

TIA.

Dan
 
I'd use a well-placed G52 Z.010; line before cutting, each tool with this orientation. (or G52 Z0.25 if programmed in metric). Cancel at the end of the tool with a G52 Z0.0;
 
Hi guys,

Would appreciate your help with something as I haven't been machining very long, so my experience if not as great as most of you on here.

I have completed a job previously (a batch of parts) have a proven program on a VF4 Haas that uses 4Axis. I have been asked to leave on 10 thou / 0.25mm to each side of this part (so part will sit higher on the fixture plate) to allow for skimming / any errors. The part is therefore sitting 0.25mm higher on the plate, and the very top face of the part is therefore 0.5mm higher than intended. The program has essentially been written long hand as no CAD/CAM.

How do you think it's best to adjust the heights? I cannot simply put a 0.25mm tool offset in because some tools are used in multiple A axis angles.

Any ideas for resolving this would be greatly appreciated.

TIA.

Dan
Hello Dan,
If this is to be a permanent arrangement, actually write the finish allowance into your part program. If only a one, or few off arrangement and the same tool is used where 0.25mm is to left in some areas and not in others, use different Tool Offsets in the various, respective areas.

Regards,

Bill
 
Hi,

I hadn't thought of that! It will still be quite painstaking, but I think will be the way to go. Means I can pick and choose where to place the datum shift, so same tools can either have it or not, depending on the angle. Thanks!
 
Stuck..good to call a tow truck..a Ford or Chevy might be Ok.. A Diamond Reo would be best but they don't make them anymore. I thought they went out of production about 1950 or so, nut now I see later models.

The History of Diamond Reo Trucks – Part I |

Horses don't often get stuck so can sometimes be better than a tractor.

*A good thread title makes a future search possible.. A key asset to a good tooling website..That is very important.

Otherwise, all is just hen's chatter,.
 
Stuck..good to call a tow truck..a Ford or Chevy might be Ok.. A Diamond Reo would be best but they don't make them anymore. I thought they went out of production about 1950 or so, nut now I see later models.

The History of Diamond Reo Trucks – Part I |

Horses don't often get stuck so can sometimes be better than a tractor.

*A good thread title makes a future search possible.. A key asset to a good tooling website..That is very important.

Otherwise, all is just hen's chatter,.

What ARE you on about!? :crazy:
 
What ARE you on about!? :crazy:
He is talking about your thread title. it is not informative about what your problem is. Thread titles like yours usually get locked pretty quickly. Just a word of warning for future post from you.
 
Hi All:
Does anyone else see a colossal clusterfuck looming on the horizon here?
I'm talking about the bodge used to get a part off the mill with the new requirements... not the thread title.

The OP says it's a repeat part using a "proven" program that he's now going to do a crazy jigger with in the hope that he gets it all mentally correct and can somehow get a usable part off, with some new stock allowance; all presumably so he doesn't have to re-program the part.

In addition, there's only a very small shift over multiple tools required (and only for some operations), so it's not immediately obvious if he's programmed a move wrong...he'll only find out when the part goes to inspection or when there's a crunch.
I get that the part is hand coded, I get that he (or someone in management) doesn't want to invest the time it takes to do it the more foolproof way, but I also know that every time I've tried something like this I've regretted it sooner or later.

I predict a crash or at least a fucked up part...if it works out good in this instance I will be happy for the OP, and I will cheerfully eat crow and admit I was wrong.
If I'm right I will try not to say "I told you so".

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Oh the actual problem..

If it is a reoccurring job I would re dimension the print to the plus .010... but I am not the CNC guy*.
That way one can see the relationship to other features and not just adding size in the wrong places.

(*except for CNC grinders)

Yes for the title we should scrap this thread and start the same with a proper title

"How to add finish size to a CNC part program." might be Ok.

It is an important/interesting subject...parts changing in heat treat and needing finish grinding is one problem needing careful watching size...at one shop we had a book that told the expansion and reduction to various metals (steel) so we could better figure size after heat treat. I also was given the sheets on carbides formulas/mix from one carbide manufacturer, likely worth big bucks today..yes I destroyed them.
 
Hi Scoop:
You wrote:
I do not have access to CAM software :-)

You have my profound sympathy.
I don't know the circumstances you're working under, but that is just plain nuts in 2021: trying to make a living with CNC machines and no CADCAM in today's competitive environment.

If you pull this off you have my respect.

You also should feel encouraged to look for a better gig.
I wouldn't hesitate for a moment, to start sending resumes around.
The expectations of your bosses are not grounded in reality...you're worth more than this kind of treatment, and life's too short to be kicking yourself in the head for no reason.

Maybe I'm misreading what's going on here...for all I know YOU'RE the boss and I'm trashing on you for your own poor business judgement, but somehow that's not what I'm inferring from your posts.

So if I'm right in my guesses, I'd get out on the street and look for a more reasonable opportunity.
Sadly, that piece of advice is totally unhelpful for your current problem...my apologies.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
In that case, redo the program manually to achieve the same result. Don't try to fudge it with offsets, you'll screw yourself next time you set the job up. Or two years from now, when you can't remember what you did.

One can write the offset changes into their code with G10 or direct variable assignments. That way in 2 years it works the same as now.

I do that regularly with a couple widgets that I make that have morphed from the original design and program. Been doing it for 8 or 9 years now and yet to crash or otherwise eff up.
 
The way I do this is to use multiple offsets, but based on identical locations. On a 4th axis, that would be the X and Z center of rotation, with Y as the face of the rotary. The A axis offset is identical (A00) for all of them.

This offset gets copied into G54, G55, G56, etc. In CAM, each index angle where work is being performed gets one of these unique offsets. G54 is top dead center A0, G55 is A90, G56 is A-90.

This gives you an independent way to dial in each index angle to account for errors in the rotary alignment, fixture wear, etc etc. Of course, we're typically talking little tweaks of a couple of thousands here and there. To maintain those changes between runs, you can either make notes, or you can use G10 at the top of your program.
 
I'm with beege. No need to over complicate things:

( PROGRAM HEADER AND JUNK)
G52 Z0.
#800=.01

G52 Z#800 (Insert this before any code running at needed A axis positions)
CODE (Do super cool stuff at said A axis position)
G52 Z0. (Insert this after to cancel so it doesn't effect other A axis positions or other work offsets)
 
I like the variable approach, too (my machine wasn't purchased with that option turned on) With the variable, you could then raise or lower Z using the G52 line, Then after a 90° index, shift Y by the same amount to move any side geometry in a similar fashion
 
A little "finger cam" and calculator practice is good for the brain anyhow, make a copy of the program, just in case you F..up then fix it.

Find a moderator to help you fix the title, you may be the one trying to search it one day
 
I'm with beege. No need to over complicate things:

( PROGRAM HEADER AND JUNK)
G52 Z0.
#800=.01

G52 Z#800 (Insert this before any code running at needed A axis positions)
CODE (Do super cool stuff at said A axis position)
G52 Z0. (Insert this after to cancel so it doesn't effect other A axis positions or other work offsets)

Hi,

Thanks for your suggestion, I am new to the world of Macros, would you mind expanding on this, what it does exactly, how to implement it and so on?

Thank you,

Dan
 








 
Back
Top