Please do. Seriously!
Fadal Toolsetting method
- Thread starter Cole2534
- Start date
Barbter
Well-known member
So....I appreciate there's 10+ ways to set tools....when I was Eng Mgr at a place, the Leadwell cell were set from Z home.If you already have a Haimer the very best thing you can buy to accompany it is one of these (picture below).
I have 3 or 4 of those on the shop floor, along with some fancier Nikken ones that I use on the mills usually, but they are way more expensive and not necessarily better.
On the Fanucs I dedicate G58 to tool setting, although on smaller machines you can just use any work offset that is zeroed. I use G58 because zeroed doesn't work on larger machines as Fanucs can't accept a tool offset larger than 999.999mm. I digress.
Set the haimer on the reference edge and tools on the plunger. Then use the Haimer to set the work offset on the part. If you have a work offset dedicated to setting tools, just call it up whenever and set tools without affecting anything else.
So tool length numbers were massive.....
Where the Hitachi cell was set so the tool length was gauge to cutter tip (to me = sensible).
Matsuura cell had probes etc....
For my place, we only set the Hitachi way above - using a100mm toolsetter (similar to above), which could sit anywhere on the table, and all I ever did was zero the spindle nose first (no holder in spindle) and then call the T# and bring the tool down on to it.
This allowed no changing any datum, and then because all tools were set relative to eachother (because they're all from the spindle nose), it allowed next job to be set (new G54 or 55 etc) and all tools could be used with no tool resetting.
But it's the only way I know!
Last edited:
The problem I've had for this is that my CAM (F360) applies the fixture offset in a way that will overtravel the Z when it's applied. If there's a way around this I'd love to see it.
Watch T-dubs video. My tools on a Fadal are not relative to the part in any way, it's setting myself up for a crash. Mass modify is a useful and unique option on a Fadal. BUT tools length should be relative to themselves not the part. The E value (G54 in common speak) is coordinate data, not Tool data. Sometimes I use E1-8 in the same slamming shut of the doors, I couldn't do that if the Tools were relative to the E value.
E
E
I forgot to say that I use F360 as well and I've never had an issue.
A lot of times I have a system that works for me. One example is when I'm running a lathe, I don't use a pre-setter. I don't care how expensive it was or if it's Renishaw's most updated foolproof dick sucking wazzoo thingy majig.....but I remain slower than other guys because of it. I don't teach guys to stop using what works for them. Another one is, when I'm using an old spinny edge finder, I jog up on Z before I enter any values at the control. Totally arbitrary, but it works for me. If what you're doing works for you do it. But if you started a Thread to learn a better/easier/faster way...you've got some good start points!!
R
R
Herding Cats
Hardplates
Is your post calling the tool offset and first z move in the same block? If it calls the offset alone at a Z home location this can cause a machine to OT.
I'm out of the shop today. I'll check back and post a code snippet.
That's exactly what it does. Guess I need to learn to modify my post...
Attachments
Herding Cats
Hardplates
I know on a Fanuc OT there is a parameter that determines if the machine moves on a tool offset call or if it waits for the first block that moves the axis.
Something worth researching if you don't want to fool with the post.
Most controls are much more customizable than people realize
Something worth researching if you don't want to fool with the post.
Most controls are much more customizable than people realize
Barbter
Well-known member
Parameter 5002?
Herding Cats
Hardplates
14.4 on an OT. I think the OP has a Fadal so I won't we of any help with parameter numbers.
atex57
Member
- Joined
- Mar 31, 2021
- Messages
- 78
- Reaction score
- 63
- Location
- SW Wisconsin USA
- Website
- Fanta-Machine.com
To the OP whom I think is TheOldCar, how I set tools on my Fadal. Also watch TDubs video.
After CS, Cold Start
Press Manual to get to Enter Next Command
Press DT, Display Tools
Press 4 Utilities
Type in the numbers of the tool(s) you want to set
Press 1 Jog
Enter the height of the block you are measuring from, I use a 2" block so I put in 2.0
Press Start
Press 1 to input tool diameter
Press 2 to locate length
Jog to a good position on the table and jog the tip of the tool lower than the height of the block, then slide the block against the tool and jog up until it slides under,
use the increment selector to get the closest fit.
When you have a good fit to the block then press Manual or Start depending on the number of tools you are setting. Rinse and repeat until done.
This way all tools are set from a common place, the table, and all workpieces are also set from the table using fixture offsets found in DF, Display Fixtures and called by the E numbers.
Any questions? You got a handle on fixture offsets?
Ed.
After CS, Cold Start
Press Manual to get to Enter Next Command
Press DT, Display Tools
Press 4 Utilities
Type in the numbers of the tool(s) you want to set
Press 1 Jog
Enter the height of the block you are measuring from, I use a 2" block so I put in 2.0
Press Start
Press 1 to input tool diameter
Press 2 to locate length
Jog to a good position on the table and jog the tip of the tool lower than the height of the block, then slide the block against the tool and jog up until it slides under,
use the increment selector to get the closest fit.
When you have a good fit to the block then press Manual or Start depending on the number of tools you are setting. Rinse and repeat until done.
This way all tools are set from a common place, the table, and all workpieces are also set from the table using fixture offsets found in DF, Display Fixtures and called by the E numbers.
Any questions? You got a handle on fixture offsets?
Ed.
Thanks for the walk through, worked perfect.