Category Archives: Siemens Mill

Writing Siemens Work Offset From Your Program

Category : Siemens Siemens Mill Siemens Turn

Writing Siemens Work Offset From Your Program

Siemens Work Offset

On a Fanuc control it is quite common to use G10 to write your work offsets (G54 to G59) from your program. It has many advantages the main one being that no-one gets to mess with your precious work offset once its set.

 

If some prick comes along and changes it, you don’t have to give a flying monkey shit. Your Siemens Work Offset is safely locked away in your CNC Program.

Oh and you get to do shit like this

Well if you ever lie awake at night thinking “how is that done on a Siemens control” I’m going to give you the answer. I often had these thoughts so you are not alone.

But then one day, not long back, someone asked me outright “How’s it done” once I got over the initial embarrassment of being asked such a direct question I told em.

Well first let’s say there is no such thing as G10 on a Siemens control.

You use this $P_UIFR[1] to write your Siemens Work Offset. The 1 being G54 and 2 G55 you can take this right up to G599.

Beware you are in the adult section now, messing with system variables.

Let me say “I fuckin love Siemens controls” there you go I’ve said it.

But, and a massive but it is, you get the syntax wrong on this and all hell will break loose. Not only will your CNC Machine explode in your face but when you get home your partner will be shagging the window cleaner in the remains of your burnt down house. So beware before you press that button to write your Siemens Work Offset.

You need loads of commas just put em everywhere and you wont go wrong.

This is how it looks:

$P_UIFR[1]=CTRANS(X,100.,Y,200.,Z,300.)

This will set X100. Y100. and Z300.

Great I Can Read and Write

While we are on the subject, you can also read the work offset figures back into R values. You can then keep these and do what you want with them. Maybe sell them to a friend for profit, the choice is yours.

Siemens Work Offset

The 1 just after the square bracket is for G54 (2 would be G55) then give the axis in our case X Y and then Z

R1=$P_UIFR[1,X,TR]

R2=$P_UIFR[1,Y,TR]

R3=$P_UIFR[1,Z,TR]

The video below shows R1 R2 and R3 set to zero, after reading the program it extracts the offset figures G54 X-100. Y-200. and Z-300. and puts em in R1 R2 and R3 variables.

So there you have it setting you Siemens Work Offset.

Easy isn’t it.

You’re a big boy now playing with system variables but just remember “with great power comes great responsibility”

 

 

 

Save Offsets Siemens 828

Category : Siemens Siemens Mill Siemens Turn

Save Offsets Siemens 828, I often see my job as a trainer as the bloke who works out what those odd buttons do. You know, the one you see every day but never dared press it because it might cause your machine to implode and completely destroy itself.

As you know I offer on-site training on all types of controls.

Well I was messing with a customers machine today and found another, button that is.

Save Offsets Siemens 828

Save Offsets Siemens 828

This is the chappie his name is Archive but he does other things other than what it says on his tin so to speak.

If you dare to press him you have the luxury of being able to save all your offset and tools related to your program and you will be blessed with special powers, a bit like Spiderman but without all those sticky bits of thread.

“How cool is that”

What you Do to Save Offsets Siemens 828

First of all you will need to be in Program Manager.

You should then be able to see this screen.

Save Offsets Siemens 828

Now press the button.

You will now have the option to press

Save Offsets Siemens 828

So go ahead press it.

From the dropdown boxes you can chose what you want to save.

Save Offsets Siemens 828

Press OK and everything will be saved in a file which has the same name as your program flowed by TMZ. Not sure what that means but it contains all your shit.

So that’s good (Save Offsets Siemens 828)  isn’t it?

It has the extension INI.

My program was FACEMILL so it added FAEMILL_TMZ.INI

So now it’s easy. When you want to recall this information just open the file (much like you open a program) and there it is.

Save Offsets Siemens 828

 

Just click OK and your data is all reloaded.

Save this file with your program and everything you need is there. Don’t you just love that??

I know I do.

This is Storm, a friend of mine. He’s only a boy but when he grows up he’ll be a tiger.

Sorry but did I mention my 5 star reviews?

I really am far too shy to do this but the wife will kill me if I don’t.

Haas VF3

 

 

 

Siemens 810d REPOS, are You Repositioning?

Category : Siemens Mill

This article is about the Siemens 810d REPOS key.

I am so lucky that I get to meet so many fascinating people. Recently I worked at The National Oceanography Centre.

These guys do all sorts of scientific research shit. Most of it I don’t really understand but I do know they have their own ship and they go out to sea taking samples and fixing stuff.

This is what they say they do:

We provide industry with innovative solutions to their problems, train the engineers and audiologists of the future, and impact on society through our world-leading research.

Oh and they have this baby:

Siemens 810d Repos
Hardinge VMC 600

It’s a Hardinge VMC 600 and it’s got a Siemens 810D control and I love it. I definitely get too attached to the machines I work on and this one is no exception.

A bit grubby at the minute but they assure me she’s gonna get a makeover soon.

I Hate Celebrities

Tonight I’m stuck in my hotel room and the only thing on the telly is a load of Z list  celebrities competing to see who can make the best frittata. This gives me a problem in that I hate celebrity culture and I don’t have a clue what a fuckin frittata is.

Oh and on the other channel it’s celebrities on a games show crying cos they couldn’t win two thousand pounds for their chosen charity. I mean, fuck off , these guys spend five hundred quid on a pair underpants and could donate twenty grand to a charity without batting a surgically lifted eyelid.

Enough About Celebrities

Having not worked on this Siemens 810d control for a little while a few things had slipped my mind but it didn’t take long to get back up to speed.

Thanks for sending us the manuals YeovilMachine Tools YMT (within a couple of hours) not bad eh?

This machine is 15 years old and I would put it up against a lot of new machines for ease of use and just about everything.

Graphics Mmmmm…..

The graphics, as usual, are an absolute pile of dog-shit. But honestly what machines do have good graphics even new ones?

Don’t you just love em?

I mean graphics, they kind of serve a purpose in that you know that you are somewhere near what you want. Unfortunately that’s where it ends I’m afraid.

Anyway what is this self opinionated prick going on about today? You may ask.

Well………

It’s the Siemens 810d Repos Key

If you use this REPOS button all the time and you know what it does then you are on the wrong website. Clever people like you don’t belong on this website.

 

 

Yes this is it the Siemens 810d Repos

I’d just forgotten how useful this is so you will forgive me for getting really excited about it.

The great thing about being old, and there aren’t many, is constantly forgetting things. I know that sounds weird but you can get excited about something you already knew but forgot.

The button for fuck sake let’s hear about the button.

OK the button.

So you milled half way along a part and you want to have a look at it before you go on and possibly scrap the part.

Here Is what You Do

Hit CYCLE STOP, that’s this one….

It will oblige by lighting itself up. Now you can go into manual or jog depending on the age of your machine.

Siemens 810d Repos

Now move your X Y or Z anywhere you want so that you can have a good look at the part. Maybe check it or something?

You will need to stop the spindle if you want to open the doors.

Then when you are happy to carry on just hit CYCLE START button.

Siemens 810d Repos

If you’re thinking “hang on Dave, you didn’t switch the spindle on”

Clever Siemens 810d

First of all don’t call me Dave, I fuckin hate it, my name is David. Actually you don’t need to switch on the spindle, clever old Mr Siemens just does it anyway.

Your tool will just move straight back to where it was n carry on.

“But Dave what about REPOS”

Please stop calling me Dave or I’ll end this article now and you’ll never know.

The problem is that although the control is clever enough to know it’s got to go back to where it was before it carries on.

It will still hit things on the way like this.

So what do we do?

Yes we use REPOS

Siemens 810d Repos

Then we can separately move each axis back in whatever order we want.

Don’t worry if you get the direction wrong, it will only move in the correct direction and also the correct distance.

Each axis moves back to it’s original position with no fuss. Then when you’re ready.

Turn off the REPOS and press CYCLE START.

Siemens 810d Repos

You actually press JOG to switch off REPOS which is a bit strange but once you are used to the logic (if there is any) it’s just fine.

Siemens 810d Repos

On my machine the JOG button says Manual, I think Hardinge made their own button for this. Probably from recycled pubic hair.

I’m all for reducing carbon foot print n stuff but I prefer good old JOG.

Siemens 810d Repos

I did warn you the machines not clean yet.

So this is how it works

 

Not painful at all.

We do loads of Siemens training at the CNC Training Centre

 

 

 

Siemens 840D Circles G02 G03

Category : Siemens Mill Siemens Turn

Siemens 840D Corner Rads and Circles

Siemens 840D

Siemens 840D. When I was at school they taught us, among a few other things, the rule: I before E except after C.

Click here for Siemens training.

Well I never took it in because I can never remember how it works with Siemens. Anyway let’s forget spelling bollocks and get on to the exciting stuff of CNC Programming.

Siemens 840D is an amazing control it’s so versatile. I honestly think that if you could find the right G code it could make you a one shot skinny latte with a shot of caramel syrup. No I’m joking it obviously can’t add syrup.

This article is about circular moves on the Sinumerik Siemens 840D.

Now we all know on a Fanuc it’s end point and rad (piss easy you say) and Heidenhain, well they have a lot of ways too actually.

The Germans have got this circular milling business fuckin nailed.

Siemens 840D

Gadgets

When you’re a real geek like me you just keep looking for more and more things that a control will do.

On the Sinumeric Siemens 840D it’s never ending.

Sometimes I think “shit that’s amazing” and even though I can’t think of a use for whatever it is I found. I can’t help but think maybe one day I will. You know like that bread making machine you bought that’s at the back of the cupboard.

But it’s like they cover every option and permutation you will ever want.

For example this video shows how you can simply add a radius to a corner. You just program it point to point. It’s a 50mm square so you program it to X50. Y50.. Then when you want rads on the corners you just stick them on the end.

The smart arses are now saying “so what, I can do that on my Fanuc”. (I say “good luck with that one”)

Heidenhain is easy you just add RND

Ok so here is a video showing you how.

Type 1 Corner Rounding Siemens 840D

Now I know what you’re thinking (“so what”). But what if you wanted a different feed-rate on the corner radius?

Easy just add FRC=50.would give you a feed of 50mm per minute just on the corner radius and it wouldn’t affect your other feed.

Stay Tuned It Gets Better

So your program looks like this

G41 X0 Y50.
X50. RND=20.
Y-50. RND=20.
X-50. RND=20.
Y50. RND=20.
X0
G40 X0 Y65.

Simply add FRC

G41 X0 Y50. F200.
X50. RND=20. FRC=50.
Y-50. RND=20.
X-50. RND=20.
Y50. RND=20.
X0
G40 X0 Y65.

Oh and if you want it to apply to every corner you don’t need to write one on every line just add M. Cool what.

G41 X0 Y50. F200.
X50. RND=20. FRCM=50.
Y-50. RND=20.
X-50. RND=20.
Y50. RND=20.
X0
G40 X0 Y65

Oh and you can do the same with the RND just add M

G41 X0 Y50. F200.
X50. RNDM=20.
Y-50. 
X-50. 
Y50. 
X0 RNDM=0
G40 X0 Y65

Then RNDM=0 will cancel it.

Type 2 Endpoint and Radius Siemens 840D

This is how you do it just like Fanuc n Haas

 

 

I mean really it’s not much different to fanuc and Haas except instead of just putting R20. you have to put CR=20. these Siemens guys love those equals signs they seem to want them everywhere.

Type 3 Tangential Rads Siemens 840D

I love this one (Heidenhain do it too) all you do is give it two points and it just sticks in a tangential rad.

Oh by the way if you think there is more than one size tangential radius between two lines then you should be absolutely ashamed of yourself.

It’s all done with a simple CT don’t you just love it this is soo damned exciting.

Type 4 Angle Siemens 840D

This one is amazing you just program a radius and the angle.

Type 5 Using I and J Siemens 840D

 

Siemens 840D

Proceed At Your Own Risk

As much as I don’t like to swear in my articles I’ve got to say I fuckin hate I and J as a way of circular interpolation.

There I’ve said it.

It’s pointless, it’s outdated and it’s utter bullshit.

The only time I would ever use I J and K would be to machine a full circle. Other than that I would rather extract my own wisdom teeth with a hammer and chisel.

 

There it is. The I and J are an incremental distance to the centre of the circle from where you are. Oh and because Siemens is so versatile you can even program I and J as absolute values from your datum.

If you find the above statement confusing then good. It serves you right for using a completely useless outdated way of programming a simple corner rad.

So now you know what I mean. Joking aside, these methods are all tools in your programming toolbox. One day you’ll see a use for one of them and you’ll think “I remember that grumpy old bastard wrote an article on that”.

Then I hope you’ll return to this article.

Thanks for watching and reading

If you have been affected by any of the issues in this post or need CNC Counselling then contact me.

Or call us

If you want to learn to program CNC Milling Machines

Look no further Contact CNC Training Centre

 

 

 

 

Onsite Training

Careers in CNC

View all current vacancies in CNC

Click here

Classroom Courses

Apply Now

Call David: 07834 858 407

© Copyright 2020. All Rights Reserved