Mazatrol Matrix Nexus - Unwanted Taper in BAR OUT

Isak Andersson · Nov 3, 2021

Hello. I'm getting some weird results when I try to simulate my program. It looks like it's cutting a taper in the X direction but only in BAR OUT. All other operations look fine. It does look straight in SHAPE CHECK but not in TOOL PATH or VIRTUAL MACHIN. What could possibly be the explanation for this?

Here's the program:

It also makes some funky-looking chamfers on the ID. The 0.2 chamfer is not at 45 degrees and it adds chamfers on the inside of the corners which I don't want. What's going on there?

Isak Andersson · Nov 3, 2021

It didn't let me upload more than 5 images so here's the program for the ID.

CNC Hacker · Nov 3, 2021

It's from the "CUT ANGLE" and "EDGE ANGLE" settings for the tools you're using in tool data. Mazatrol will look at those angles to figure out where it can fit the tools and still have clearance. It wants like 2 degrees of clearance to the backside of the insert. So if your cut angle is set to 90 degrees it will put a taper on shoulders instead of plowing the tool into it.

Isak Andersson · Nov 3, 2021

Thank you. I did have exactly 2 degrees of clearance but I increased it to 5 degrees and now it works.
Do you know what's going on with those weird chamfers tho?

Philabuster · Nov 3, 2021

Isak Andersson said:
Hello. I'm getting some weird results when I try to simulate my program. It looks like it's cutting a taper in the X direction but only in BAR OUT. All other operations look fine. It does look straight in SHAPE CHECK but not in TOOL PATH or VIRTUAL MACHIN. What could possibly be the explanation for this?

Post up your tool data page. It sounds like you do not have your tools geometry described correctly.

Gobo · Nov 3, 2021

Agree. Definitely a tool data issue. When in doubt, describe your tool as SPT or NO TOOL, whatever option it is that your control will give you.

Isak Andersson · Nov 4, 2021

Philabuster said:
Post up your tool data page. It sounds like you do not have your tools geometry described correctly.

Philabuster · Nov 4, 2021

Isak Andersson said:

Why do you have tool ID as "G" and "F"?

On my Integrex with the Smooth X control, if the tool ID is not correct, the machine will not make good parts. For my machine, OD turning tools are ID "B" and boring bars are ID "A". I do not know if it would be the same for your machine.

The tool angles are set correctly though, so I do think it is the tool ID messing with you.

Also, on the tool nominal description, I usually set the tool number as the nominal diameter for turning tools and boring bars. You do not have any value in the OD turning tool for nominal.

Isak Andersson · Nov 5, 2021

Philabuster said:
Why do you have tool ID as "G" and "F"?

Well, the idea was to differentiate the roughing tools from the finishing tools. F being finishing and G being roughing.

Philabuster said:
The tool angles are set correctly though, so I do think it is the tool ID messing with you.

What do you mean? How would the ID make any difference?

Philabuster said:
Also, on the tool nominal description, I usually set the tool number as the nominal diameter for turning tools and boring bars. You do not have any value in the OD turning tool for nominal.

That seems like a hacky way of doing it. I didn't enter a nominal diameter of the external tools because they don't have a diameter. I guess I could enter the width of the shaft as the "NOM." but it doesn't seem to make a difference in the simulator either way.

Philabuster · Nov 8, 2021

Isak Andersson said:
Well, the idea was to differentiate the roughing tools from the finishing tools. F being finishing and G being roughing.

What do you mean? How would the ID make any difference?

That seems like a hacky way of doing it. I didn't enter a nominal diameter of the external tools because they don't have a diameter. I guess I could enter the width of the shaft as the "NOM." but it doesn't seem to make a difference in the simulator either way.

The ID letter determines the tool orientation to the machine. It is not just an arbitrary letter.

The "hacky" way was instructed to me by several Mazak Apps guys when I was learning how to run the Integrex.

Gobo · Nov 8, 2021

Maybe hacky means something different in Sweden than in the states. :eek:

Isak Andersson · Nov 9, 2021

Philabuster said:
The ID letter determines the tool orientation to the machine. It is not just an arbitrary letter.

The "hacky" way was instructed to me by several Mazak Apps guys when I was learning how to run the Integrex.

Are you sure about that? I'm reading the operating manual right now and this is what it states:
"NOM-⌀/NOM. mm(in.) Nominal diameter or nominal size of the tool"
"ID code - Suffix (Code that identifies tools of the same nominal diameter)"

You show me where in the manual it states that the ID determines the tool orientation or that the NOM. should be used for tool number. In my world, "nominal" refers to dimensions. Not sure how that relates to tool numbers.

You know, maybe those "Mazak Apps guys" were wrong or maybe you misunderstood what they meant. Just saying.

CNC Hacker · Nov 9, 2021

ID code was important on the older (MKII and MKIII) Integrexes for determining the tool orientation and B axis angle. Now it is basically arbitrary, whatever makes sense to you for differentiating between tools. I've used A for head 1 and B for head 2, R for rough, F for finish, A for alumninum, etc. The machine won't care either way.

Nominal name for turning tools is also arbitrary. I usually like to use the insert angle for the name, so an OD 80 degree tool would be "GENERAL OUT 80A" or something along those lines. A lot of people will set the nominal to the tool station number, which also works fine. I personally like being able to tell at a glance which tools are where on the turret/magazine.

Isak Andersson · Nov 9, 2021

Alright. Thanks for clearing that up. I do find it confusing, tho, if it uses nominal diameter for tools like drills and end mills but uses tool numbers for other tools. The lack of consistency makes it very unintuitive in my opinion. Insert angle makes more sense to me but then how do you differentiate between front-facing and back-facing tools if they both are described as general out? Different ID codes, maybe, or how would you do that?

I did notice the control will automatically tell apart back/front-facing boring bars (general in), tho, but not external tools (general out). What is the reason for this?

Search

Largest Manufacturing Technology Community on the Web

Search

Mazatrol Matrix Nexus - Unwanted Taper in BAR OUT

Isak Andersson

Aluminum

Isak Andersson

Aluminum

CNC Hacker

Cast Iron

Isak Andersson

Aluminum

Philabuster

Diamond

Gobo

Titanium

Isak Andersson

Aluminum

Philabuster

Diamond

Isak Andersson

Aluminum

Philabuster

Diamond

Gobo

Titanium

Isak Andersson

Aluminum

CNC Hacker

Cast Iron

Isak Andersson

Aluminum

Similar threads