Z-Axis Hitting Limit Switches as the Start of a Cycle

PartScrapper9000 · Nov 14, 2018

I have been having this issue for a while and have just been dealing with it, but I figure its probably time to ask for help. Excuse my formatting, this is my first post.

As I said in the title, at the start of all tool paths, the machine goes up to z15 and crashes into the limit switches. Every time I have to jog the machine back down then run the next line.

The line that appears to be causing this is "G43 Z15. H1"
I can't figure out why the CAM software (Fusion 360) would try to do this as I have not seen this occur on other machines. Although other machines I have seen were not using Fusion 360.
I am running mach 3 by the way.

Is this to do with the clearance and retract heights and is this normal? Additionally, will deleting the line have a negative effect on the tool path?

Thanks in Advance!

Booze Daily · Nov 15, 2018

It's either clearance/retract height set to the tool in your CAM, or you set your tool lengths off the face of the part giving you a large negative tool offset with a G54 Z set to 0.
Or a combination of both.

DMF_TomB · Nov 15, 2018

PartScrapper9000 said:
I have been having this issue for a while and have just been dealing with it, but I figure its probably time to ask for help. Excuse my formatting, this is my first post.

As I said in the title, at the start of all tool paths, the machine goes up to z15 and crashes into the limit switches. Every time I have to jog the machine back down then run the next line.

The line that appears to be causing this is "G43 Z15. H1"
I can't figure out why the CAM software (Fusion 360) would try to do this as I have not seen this occur on other machines. Although other machines I have seen were not using Fusion 360.
I am running mach 3 by the way.

Is this to do with the clearance and retract heights and is this normal? Additionally, will deleting the line have a negative effect on the tool path?

Thanks in Advance!

.
obviously if G43 Z15. H1 is stated the spindle face is higher by the tool comp amount.
.
if you got a 10" tool and H1=10.0 than the spindle face is trying to go to Z25. if machine wont go that high it will alarm out obviously

HuFlungDung · Nov 15, 2018

For general machining operations carried out with the part in a vise or on the table (as opposed to a 4th axis), the part zero is best kept at the top of the part. This way, any machine movement while the tool is at a positive Z position should be in clearance (except for clamp components). So then, you don't have to have a huge Z+ value to be 'safe' above the part. What you have there looks like a 'safety line of code' to me, but it has not been configured in value to suit your machine/circumstances. You should be able to edit that value somewhere in your post settings.

DMF_TomB · Nov 15, 2018

often called initial Z or safe clearance over part to not hit part or clamps.
.
often 2" above part and or clamps so operator can see collision not going to happen
.
you usually set initial Z or tell CAM program what to use. often you might need initial Z of 3" if part top is zero and clamps stick up over 2" above part zero
.
if you got a extra long tool like a drill bit you might need to limit initial Z as machine might have limits on how high it will go
.
some programs tool change arm with a long tool in it will hit vise. if it wont go higher the vise is moved far enough away in X and Y to clear tool change arm

Dan from Oakland · Nov 15, 2018

In Fusion in your 1st operation, go to the "Heights" tab and check where you have your "Clearance Height" set to. As stated above- its pretty normal to set this value to 2" or 3" as this is a safe distance giving you a sanity check on your tool offset when you run the program and to clear any fixtures or clamps. I suspect that 15" value in your program is coming from there in Fusion- what is your next Z rapid move in the program- it should be whatever you have the "retract height" or "feed height" set to in your Fusion operation for that tool.

PartScrapper9000 · Nov 16, 2018

Thanks for the help, I think I understand that problem now.

I am also having issues with toolpath generation in mach 3 and well as the z-axis plunging.

The z-axis plunge issue is similar to what I outlined originally except when the code specifies Z0 the machine plunged to z40 - straight down into the work piece. This does not seem like a CAM issue to me.

With the tool path generation, I have a rectangle shape pocket that I am cutting with a 2D apative tool path but not even half the rectangle is showing in mach 3 (when the code runs this is the result too). I loaded the same G-code on mach 3 on another computer and it loaded correctly. The computer that I am running it on is running windows XP, a fully licensed version of mach 3, but has integrated graphics. Does anyone know what the issue could be here?

Sorry for going a bit off topic here but I figure its somewhat related and easier than starting a new thread.

PartScrapper9000 · Nov 17, 2018

Thanks for the help, I think I understand that problem now.

I am also having issues with toolpath generation in mach 3 and well as the z-axis plunging.

The z-axis plunge issue is similar to what I outlined originally except when the code specifies Z0 the machine plunged to z40 - straight down into the work piece. This does not seem like a CAM issue to me.

With the tool path generation, I have a rectangle shape pocket that I am cutting with a 2D adaptive tool path but not even half the rectangle is showing in mach 3 (when the code runs this is the result too). I loaded the same G-code on mach 3 on another computer and it loaded correctly. The computer that I am running it on is running windows XP, a fully licensed version of mach 3, but has integrated graphics. Does anyone know what the issue could be here?

Sorry for going a bit off topic here but I figure its somewhat related and easier than starting a new thread.

precisionmetal · Nov 17, 2018

I assume this is some sort of router? You are using the correct post for Mach3, yes?

PM

PartScrapper9000 · Nov 17, 2018

precisionmetal said:
I assume this is some sort of router? You are using the correct post for Mach3, yes?

PM

Yes the post is definitely correct, and I am using a 3 axis CNC Router.
Everything else runs smoothly and the code works correctly when run on another computer, so I don't think it's an issue on the CAM side.

HuFlungDung · Nov 18, 2018

IMO, these large unexpected movements are due to improper understanding of machine and work coordinate systems, and what reference surface you are using for setting/defining tool lengths. You cannot be haphazard about this, you need to really have a grasp of it.

And the catch is that all these settings occur outside of your CAM system.

DMF_TomB · Nov 18, 2018

initial Z or safe tool tip clearance height is usually the first and most important decision when starting to create a program. often this is also where rapids stop and feed is used. known many who rapid all the way close to part or vise. seen many a time mill hit vise jaws at full rapid cause when vise jaws bolted on they were up .010" from bolt hole clearance. kind of bad programming using full rapid that close to vise and clamps. bad programming even to get that close to vise jaws.
.
safe clearance height needs to take into account anything tool tip might hit when running a program not forgetting any clamps or other stuff AND tool change too. sometimes you manually have to program move table all the way over so tool change can occur without tool hitting anything

PartScrapper9000 · Nov 19, 2018

So where in mach 3 would I look for the work offsets that could potentially be causing these issues?

DMF_TomB · Nov 19, 2018

PartScrapper9000 said:
So where in mach 3 would I look for the work offsets that could potentially be causing these issues?

mach 3 i have no ideal.
.
many cam systems you can create a manual op that will put gcode at program beginning. setting default gcodes and setting work offset to certain default program starting values is common thing to do

kinetiq · Nov 30, 2018

PartScrapper9000 said:
So where in mach 3 would I look for the work offsets that could potentially be causing these issues?

There is an "Offsets" page for Mach3. It displays current work offset coordinates, displays current work offset, and buttons to select different work offsets.

Search

Largest Manufacturing Technology Community on the Web

Search

Z-Axis Hitting Limit Switches as the Start of a Cycle

PartScrapper9000

Plastic

Booze Daily

Titanium

DMF_TomB

Diamond

HuFlungDung

Diamond

DMF_TomB

Diamond

Dan from Oakland

Titanium

PartScrapper9000

Plastic

PartScrapper9000

Plastic

precisionmetal

Stainless

PartScrapper9000

Plastic

HuFlungDung

Diamond

DMF_TomB

Diamond

PartScrapper9000

Plastic

DMF_TomB

Diamond

kinetiq

Aluminum

Similar threads