Z Problems - Approaching at 0 and not offsetting for tools

[batraintech]

I'm running Gibbscam 2007, Mach3, using PostHaste with a generic Fanuc script, and on a gantry router. I made my first CNC nc code, but it has some Z problems.

The first problem is the top of the stock is .1875" but the spindle approaches at Z0. Actually in the code there is no Z at the start change. It only sets Z (to the operations R) when the XY hits the area where Operation 1 begins. My clearance plane is set at 2" in Document Control, yet it is not being used. Transitioning from Operation 1 to Operation 2 doesn't seem to use the clearance plane either. Is this a bug in Gibbs? Do I have to add it manually every time?

The 2nd problem is there is no offset when I switch tools. The 2nd tool, which sticks out more than the starting tool, doesn't get offset at all, so if I had run the code with a tool in the spindle it would have crashed into the table. This one is more frustrating because I can't find out a work around.


I've attached the file, they're custom nuts.

Thank you very much for your time.

[cadman]

Wheres the file?

[batraintech]

Originally Posted by cadman Wheres the file?

Sorry, I thought I attached it. I forgot to zip it.

[cadman]

I'll check out your file as soon as I get a chance.

[Excelmachine]

Your H numbers aren't matching your tool numbers. For example, op1, tool 3 has this line for tool control: G43 Z2. H8 . It is a general rule to have the H, which is the tool register for height, match the tool number so this line should read- G43 Z2. H3. In op 2, it is set up the same way. You are programming with T1 yet it calls out H6 which is the Z tool height register for tool 6. Might this be your problem?

[mactec54]

batraintech

I opened your VNC file & I don't know how you want to machine your part,

Have you set your tool/Tools to the top of your part,& set them in Mach tool page

Then does your tool need to step down .1875 before it starts to cut, or does it cut from the top

You have both Z numbers set positive, this can never work

So How deep do you need to drill how many holes are there, I don't have solids, so can only see/do the tee slot nut shape

[batraintech]

Thank you for the help guys, both of your suggestions fixed the problems. I didn't realize you had to have the traverse height at 0. And the tool offset is working now. It seems like all of the issues are solved. I appreciate the help greatly.

[mactec54]

batraintec

This may help as well, you had a problem with the R , were the Z would not go to the right place, this will make that happen, G83G98X---Y---Z-.187R.350Q.030F20

The G98 will move the Z up to what ever you have the Z set to in the clearance plane you had .350 it will move there, this is a safety if the R does not work