Range Error? TM1

[helocat]

Range Error? TM1

First chips yesterday on the new to us 2005 TM-1 . I loaded up a few tools, took the offsets and entered the tool information into the “Tool” page. I then tried doing a test cut using the pocket feature in the intuitive programing system. I am getting a RANGE ERROR and its alarming out. Help screen says see the maual, I have it but it does not indicate what a RANGE ERROR is. Must be somthing wrong with my offsets?

Here is what I am doing:

.188” steel plate. Pocket milling a 1.25” hole into the plate. I am using tool 3 a .500” drill for the center hole, then tool 1 a .375” EM to interpolate the hole.

For my work off set G54 at the front left corner of the work. (would prefer the back left but the instructions said use “the front of the part”.) I used a 1-2-3 block to set the X and Y, then dropped in the plate. I then set the part Z on top of the part and touched off each tool to the top of the part, all setting the height off sets.

I hit cycle start and the mill travels to the X and Y call out for the center of the hole but then alarms out RANGE ERROR.

Here are my screens and a shot of the work:



Uploaded with ImageShack.us


Pocket mill:



Uploaded with ImageShack.us



Uploaded with ImageShack.us

[L8Train]

Helocat
Dose this happen on the M3 line? You may not have set up your tools all the way in IPS. My bet is that you do not have a spindle speed or feed rate called out in the tool setup page. If the tool is not set up in IPS the control will post a "S0 M3". The Haas control will alarm out with a range error if it reads a "S0 M3"

L8Train

[double a-ron]

Change your depths to .4 not -.4. If you look at the posted code you will see - -.4 for the drill and - -.2 for the pocketing. All depths in ips are positive numbers. The probe quick code is negative though. I always thought that was funny.

[helocat]

I don’t think I called out a speed and feed as the basic instructions said not to. But I see I did not call out a material, so it might not be calculating it.

Odd on the Z depth call out to not tell it a negative number! Ok I will look at the code its posting and see what it says and make the changes.
Thank you all for your help.

Mark

[double a-ron]

I just programed your part based on your screen and as soon as it got to the line of code where there's a double - it alarms out as "range error".

[helocat]

I pulled the - out and its still doing it. I added the material type and it now shows speed and feed in the tool pages. But still doing the same alarm. Could it be that I set a G54 Z offset? I realized I took a Z offset for G54 and really don't need one right? The Z offset should be just the tool right?

For the G54 Z offset I would need to measure the length of the edge finder in the tool holder and add that to the Z offset. If I do that do I measure to the bottom of the quill?

So should I zero out the G54 Z offset? Not sure how to do that. I tried entering in 0.0 but it would not take it.

[double a-ron]

All offset #'s are incremental so if you have an offset of 4.5927 and you wanted 4.5 you would press -.0927. If you wanted 0 you would press -4.5927. Now work offsets. Yes you need one. In the code you will see g54 called out and the machine can't go to g54 Zx.xxxx with out knowing where that is. First start with your tools, lets say tools 1 and 2. First get a scrap of paper, then go to the tool 1 height in the tool offset page. Now place the piece of paper on the face of the workpiece and Jog tool 1 down in z till it just touches the paper. Press tool offset measure. Now measure the paper lets say it's .003, in the height column for tool 1 press -.003 or whatever the paper measures. Repeat this for all tools. Now go to the work offset page. Use any tool you set a height for and touch it to the face of the part. Press part zero set. Now subtract the tool height from the z work offset. Example: you used tool 1 to set your z offset, tool 1's h is 5.000. Your z work offset says -9.00. Press -5.0. Your work offset is the distance between the spindle face and your part. That is why you subtract the tools length you used to set the work offset from the z offset in g54.

My advice to you is to use ips to get a feel for how the machine functions, but start learning g-code. As the program is running single block through it with the manual open to the g code section. As it executes a line of code look up those codes to see what they do. You'll most definitely see g43 Zx.xxxx H01. That is telling the machine to use tool length offsets, go to G54 Zx.xxxx using tool 1's height (H01) or whatever tool you used. Hope this helps.

[Pondo]

Originally Posted by helocat So should I zero out the G54 Z offset? Not sure how to do that. I tried entering in 0.0 but it would not take it.

Type in the 0 and press F1 to set it. Pressing enter just adds whatever's typed in to the offset. F1 overwrites it.

[helocat]

Double a-ron Thank you good information. Once I was told how to get it to show the code so I could single block it, it was real helpful to see it read it and follow it. Its been over 12 yrs since I last read G&M code. I remember some of it!

Its almost a full week since I last ask the local Haas distributor to schedule a service and a few hrs training. I finally called Haas and spoke with their application people. Ernie at Haas was extremely helpful and talked me though it. Nice to see the quick support even though I did not by the machine new. Thank you Haas and Ernie!

First post by L8train nailed it. It the IPS set up page for the "work" did not have the type in it, so the tools then did not have the speeds and feeds in them. Thus SO M03 was it. I made the changes and then it all worked they way it should.

After a few rookie work holding mistakes (and two .375" carbide end mills) I was able to make the part. Even used the IPS engraving feature and added our company URL to the part! Whoo hoo the TM-1 is alive!

Thank you all for your help!

Mark

[double a-ron]

Yeah we bought our lathe (tl-15) used and they have always been willing to help. Allthough we did previously purchace a brand new mill and 4th axis from them.

[helocat]

Thank you to everyone! Here is my first part of our new to us mill. This is a custom transfer case mount, there will be sides welded to it and bent tubing for the rest of it.




Mark