Double checking offsets

[esadaddy]

After loading my programs I would like to double check my "work offset" and my tool offsets.

What is the small program that I can run to check them?

[stevo1]

It will depend on what your doing and how accurately you want to check. If you just want a rough eye to make sure that they are close you can just instate your tool offset and send the tool to program 0. G0G90G55X0Y0 and send Z3 and check with a 123 block.

Stevo

[esadaddy]

I got the first part,but what do you mean by send z3?

[esadaddy]

I get confused between G54 and H1

what is the difference.

[stevo1]

Originally Posted by esadaddy I got the first part,but what do you mean by send z3?

I assume you are on a machining center. If you are using for example G55 for a work coordinate then when you program G0G90G55X0Y0 this will place the tool were you want to call part 0 in X and Y. This you understand correct? If you have the top of your part set in G55 coordinates then if you were to program G0G90G55Z3 the tool should go 3" above your part. Now you can check your Z distance with 123block or a known 3" gauge. This will tell you that you have the proper Z value in G55 and your tool offset is correct.

Originally Posted by esadaddy I get confused between G54 and H1 what is the difference.

G54 is your work offset for shifting the machine to were you want your X0Y0Z0 to be. For example if you have a 1" thick part on your machine with a hole in it and you want to program from the center of the hole as X0Y0 and Z0 to be the top of the part you would find the center of the hole and put the "machine position" values in G55. So they would look something like X10.568, Y5.985, Z1.0. Now when you program G0G90G55X0Y0Z10 your machine will travel to the center of the hole 10" above your part.

The H will instate your tool length with a G43 programmed with it. As described above your spindle face would go 10" above the part. You need to have your tool active to have the tool tip go 10" above the part. So to activate your tool lenght you need to program G43H1Z10. This will take the tool tip 10" above the top of your 1" part. The H1 would use the Z value set in your offset page for T1. H2 would use T2, H3 would use T3 ect.

Some machines are set up different this can vary depending on how your home position of the machine is set up.

I don't bother with my H values when programming. I set this in my tool change program so I never have to worry about setting/using the wrong H. When a tool call is instated the length is set.

Most people dont' like to use G54 as this is typically Fanuc's default coordinate. So if you start putting values into this and you are MDI or programming and forget to put G55 if thats what your using. The machine will work using the values set in G54. So if your machine home is a safe position when programming G0X0Y0Z0 and you have values in G54 it will not go to machine home it will go to the values set it G54 regardless if you have the G54 active or not in your program.

Stevo

[esadaddy]

Well explained.

I got it now.

I appreciate the help. I have went from zero progress to fully capable in a matter of a week using this forum.

Thanks a bunch.

[stevo1]

Your welcome. I am glad you understand. Welcome aboard and the best of luck to you.

Stevo

[esadaddy]

Another question in regards to machine position.

You stated the g55 is an offset of the "machine position" How do I know I am shifting the machine position?. What I mean is that while I was able to shift the G54 column in the offset/work page, I was not able to shift the G55 column. I noticed the POS screen would shift to zero. But when I go back to the offset page and try to set the g55 column it would not move. After reflecting on this I thought that maybe I was not moving the machine position and maybe I was moving some other position.

So my question is How do I make sure that it is the machine position I am shifting.

[ALLtra Mach]

How are you setting the G54, G55? Direct input,measuring?

When you go to position "G0G90G55X0Y0", go to your "POS" screen, Your "Absolute Position" Should be X0 & Y0 as Absolute Position is controlled by your current work offset. The "Machine Position" is the actual distance you are sitting from machine home and should read the same coordinates as your G55 Offsets.

[stevo1]

Ok,
Machine home is different per machine and can be set up as what is best for the process, programming, and application of what is being done. However on most machine tools the home position is the same position as when you do a zero return at power up.

If you want to know your “home” position once you power up and do a zero return make sure you have no numbers in your common work coordinates (the ones before G54 labeled NO.00). Program G53X0Y0Z0. Where the machine moves to is your home position.

Now to use your G54-G59. You want to shift the machine from home position. So move the tool anywhere you want to in the machine as if you were trying to pick up a feature of a part on the machine. Put the “machine position” numbers into any one of your G54-G59 offsets. Move your machine off of that position. Now when programming you have to activate one of G54-G59 whichever one you want to use. So if you put the numbers in G55 you have to program G55X0Y0Z0. The machine should move to the position that you recorded and put into G55. This goes for all of the work coordinates. If you put the numbers into G58 you have to program G58X0Y0Z0. When actually programming a part you don’t need the X0Y0Z0. You just have to make one of G54-G59 modal just by programming G55. Now any XY movement will move around G55.

Don’t forget as I stated in my last post on most Fanucs the G54 is the default coordinate. If you look at your program check screen you should see the active codes and G54 should be listed after reset or program end is applied. So even though you did not active any work coordinates in your program when you tell the machine to move in X,Y,Z it will move based on what numbers are in G54.

I hope this helps.
Stevo

[ALLtra Mach]

Another thing to remember is there can be different "Machine Home" positions.
There is only one true "Reference Return" , which is the G53 position Steveo is speaking of.
You also have G28,G29, G30, G30.1 etc which although technically incorrect, are often referred to as "Home" or "Alternate Home" positions, when they are actually user controlled positions. The correct and true "Home" position is the mechanical position where that magical calculator we refer to as a "control" makes all of its calculations and movement from. This is the point a G53 will take you to, and where your "Machine Position" column will read zeros.

[esadaddy]

I believe I got it now. You guys are deep. I understand my mental error now. I was looking at the position screen assuming that that was the actual machine position but it was a already shifted position. After reading this thread again, I noticed the words "machine position" that was posted previously and I noticed the machine position column on the second page of the position screen. Then I got it.

I do 3d modeling using rhino and I am trying to produce some wax masters so that I can make silcone molds from them. So the CNC portion of my journey is very important. I have done it on a small scale using a desktop sherline and maxnc mill but after machining the same project at work on a large VMC I couldnt look back.

Also, My machine position is in mm and my program is in inch. I would like to change the machine position to display in inch. How?