megaman

Using G41.2

Recommended Posts

Hello, can anyone give me some sample code using g41.2? Is it not nessesary to hae a D  value in a g41.2 line or do i need to fix the post?

16140306920491562331556018102633.jpg

Share this post


Link to post
Share on other sites

That is 3D Cutter Compensation and I personally would not expect to see that in a threadmill toopath. Usually you see/use that in a 4+1/5-Axis toolpath in certain situations like Flowline 5-Axis, Swarf 5-Axis and Curve 5-Axis.

But since you asked;

G131F1
(5-AXIS SWARF SIDE ROUGH +.005 ON WALL)
S19966M03
M132
G00G90G54B-1.016C-5.894
G54.4 P1
G68.2 X0.0 Y0.0 Z0.0 I84.106 J-1.016 K-90.0
G53.1
X0.039Y0.1389
G69
G43.4Z0.8589H#517
X0.0379Y0.1358Z0.8602
X0.0511Y0.1344Z0.1103
X0.0537Y0.1341Z-0.0396
G01G41.2X0.0549Y0.134Z-0.1076D#517F90.0
X0.0319Y0.1232Z-0.1228

........

X0.0476Y0.1333Z-0.1088
G40
G00X0.0356Y0.1512Z0.859
G130
G00G90G49
G49G53Z0.0
G54.4 P0

Share this post


Link to post
Share on other sites

I used drill-5axis threadmill and tried to output with control comp. It shows the tool arcing to the middle  of the cutter on the edge of the hole. I coukdnt get control comp to work. Is thread milling  with 5 axis output a no-no?

 

Share this post


Link to post
Share on other sites
1 hour ago, megaman said:

I used drill-5axis threadmill and tried to output with control comp. It shows the tool arcing to the middle  of the cutter on the edge of the hole. I coukdnt get control comp to work. Is thread milling  with 5 axis output a no-no?

 

Do you  have a Head/Head machine, Table/Head, or Table/Table machine?

5-Axis drilling isn't technically 5-Axis. It is simultaneous 5-Axis or 4+1 positioning and then drilling along the Z-Axis Vector unless you're using a Right Angle Head. But It should be fine.  All depends on your machine's option package though.

I deal with Table/Table machines and typically my collision checking and post software (CAMplete) does positioning , drilling, canned cycles, etc... using G68.2

I'll have to see what kinds of parts I have and test out what I can get based on the cycle. Hang tight.

Share this post


Link to post
Share on other sites

I'll have to create something. I don;t have anything handy. Sorry.

Share this post


Link to post
Share on other sites

Yhis machine is a table trunnion machine . A mazak variaxis 730. No g68.2  on this machine.

Share this post


Link to post
Share on other sites

If this is truly an indexing situation, using G68.2 would be most desirable. That would also allow the use of standard cutter comp, G41/G42.

  • Like 3

Share this post


Link to post
Share on other sites

How does Mazak get away not having G68.2 on a 5 axis machine?

Share this post


Link to post
Share on other sites
1 hour ago, PAnderson said:

How does Mazak get away not having G68.2 on a 5 axis machine?

By using g54.2 p.... dynamic offset

Share this post


Link to post
Share on other sites
On 2/23/2021 at 7:09 AM, megaman said:

Yhis machine is a table trunnion machine . A mazak variaxis 730. No g68.2  on this machine.

No G68.2 on the machine? Or no G68.2 in the post?

Share this post


Link to post
Share on other sites
On 2/23/2021 at 4:09 AM, megaman said:

Yhis machine is a table trunnion machine . A mazak variaxis 730. No g68.2  on this machine.

No Option bought for it might be the case. They support G68.2 with their G68 with no issues. Question is do you have the right post and have you do the correct testing of that post to vet it for your machine?

Share this post


Link to post
Share on other sites

 

2 hours ago, So not a Guru said:

No G68.2 on the machine? Or no G68.2 in the post?

 

22 minutes ago, crazy^millman said:

No Option bought for it might be the case. They support G68.2 with their G68 with no issues. Question is do you have the right post and have you do the correct testing of that post to vet it for your machine?

Hi guys, 

 

you are correct it may be that we just don't have that in our post. I have been programming this machine for years but only diving into the full 5 axis more that I have ben programming full time. I haven't had issues with this post too much but I'm sure I need post refinement.  we do use g68.2 on our head  table machine (VTC800).  the multiaxis threadmill in drill (with control comp gives me the result below.- we always use comp to avoid changing and having operators input the wrong diameter) I was only able to get it to work by creating a plane an then using a 3 axis output and then transforming it . 

I am trying to find out whether this is a Mastercam issue or a post issue I need Inhouse solutions to modify my post. I don't see a D value and it sees to cancel at the wrong place.

 tm.png.e7ff8873aa2353b116c94cab2cf52dbb.pngtm2.jpg.85b5cdc799de418a453625fae3fadf85.jpgtm3.jpg.95cda2ecfb747e503ad487812e26684d.jpg

 

Any knowlegable input is greatly appreciated!!

Share this post


Link to post
Share on other sites
14 minutes ago, megaman said:

 

 

Hi guys, 

 

you are correct it may be that we just don't have that in our post. I have been programming this machine for years but only diving into the full 5 axis more that I have ben programming full time. I haven't had issues with this post too much but I'm sure I need post refinement.  we do use g68.2 on our head  table machine (VTC800).  the multiaxis threadmill in drill (with control comp gives me the result below.- we always use comp to avoid changing and having operators input the wrong diameter) I was only able to get it to work by creating a plane an then using a 3 axis output and then transforming it . 

I am trying to find out whether this is a Mastercam issue or a post issue I need Inhouse solutions to modify my post. I don't see a D value and it sees to cancel at the wrong place.

 tm.png.e7ff8873aa2353b116c94cab2cf52dbb.pngtm2.jpg.85b5cdc799de418a453625fae3fadf85.jpgtm3.jpg.95cda2ecfb747e503ad487812e26684d.jpg

 

Any knowlegable input is greatly appreciated!!

Well the issue is Mazak and the EIA/MAZATROL control of the tools if the machine's parameters have been set to use the MAZATROL side of the machine then you may only need the TOOL number and the D number is implied to be read. Again depending on the parameters.

What you show in that picture is probably not having simulate Control Comp on in the back plot parameters. Turn that on and that backplot will look correct. The last issue I don't use Control Comp I use wear. Just ran a program in an Integrex Yesterday and we ran WEAR with no problem and hit our desired bore since within 1 micron.  Helps then run the machine in Metric mode, but I couldn't believe we hit it that close.

Easy way to test is to take a test block and cut a hole. Then adjust the wear comp on the machine and then see if ti gets bigger it does then you don't need it. If it doesn't then add the D value manually and run it again. If it then adjusts the size that is your answer and you send that code to In-House and they will get you fixed up. Mazak's are parameter driven machines more than just about any machine out there and depending on the way the parameters are it has a huge effect on the way EIA runs on the machine.

Share this post


Link to post
Share on other sites
32 minutes ago, crazy^millman said:

Well the issue is Mazak and the EIA/MAZATROL control of the tools if the machine's parameters have been set to use the MAZATROL side of the machine then you may only need the TOOL number and the D number is implied to be read. Again depending on the parameters.

What you show in that picture is probably not having simulate Control Comp on in the back plot parameters. Turn that on and that backplot will look correct. The last issue I don't use Control Comp I use wear. Just ran a program in an Integrex Yesterday and we ran WEAR with no problem and hit our desired bore since within 1 micron.  Helps then run the machine in Metric mode, but I couldn't believe we hit it that close.

Easy way to test is to take a test block and cut a hole. Then adjust the wear comp on the machine and then see if ti gets bigger it does then you don't need it. If it doesn't then add the D value manually and run it again. If it then adjusts the size that is your answer and you send that code to In-House and they will get you fixed up. Mazak's are parameter driven machines more than just about any machine out there and depending on the way the parameters are it has a huge effect on the way EIA runs on the machine.

I am  not 100 percent sure about the mazatrol/eia settings  but  we use the actual diameter and then change that to a smaller size to get it to go bigger on internal features.

SIMULATE backplot  was on and it still does that . 

tm4.jpg.8cb463470e6466019551357e1bb19696.jpg

 

If I was going to use wear I would manually put in an m00 and tall them to make sure actual diameter is zero and use actual dia. comp to get to size. most operators just know how we normally do it.

Share this post


Link to post
Share on other sites
4 minutes ago, megaman said:

I am  not 100 percent sure about the mazatrol/eia settings  but  we use the actual diameter and then change that to a smaller size to get it to go bigger on internal features.

SIMULATE backplot  was on and it still does that . 

tm4.jpg.8cb463470e6466019551357e1bb19696.jpg

 

If I was going to use wear I would manually put in an m00 and tall them to make sure actual diameter is zero and use actual dia. comp to get to size. most operators just know how we normally do it.

You can set the Geometry Size to 0.0000, using a G10 line, or using Macro Variable Formulas in the NC  Code. Just wanted to point out that there is a method available to make sure the Operator doesn't miss making the change. In fact, you could 'save the current Geometry Size in a Common Variable, reset the Size to 0., and then restore the Size when the Operation is finished', all by using Macro Variable Formulas.

In fact, if you want to adopt Wear Comp as a standard, you could make your Post output G10 Lines in the header, to clear out all the Geometry Size values, to avoid the issue of an Operator forgetting to clear those values.

I have never been a fan of Full Control Compensation, and feel like any shop who still uses it as a standard, is basically still living in the dark ages. No offense intended...

Share this post


Link to post
Share on other sites

I don't remember the settings, but IIRC there is a parameter to use the offset register's instead of the mazatrol tool data with comp.  I also recall, although it be fuzzy that you can continue to use mazatrol tool data for the length, and only grab offset register for side comp.

Share this post


Link to post
Share on other sites
4 minutes ago, Colin Gilchrist said:

You can set the Geometry Size to 0.0000, using a G10 line, or using Macro Variable Formulas in the NC  Code. Just wanted to point out that there is a method available to make sure the Operator doesn't miss making the change. In fact, you could 'save the current Geometry Size in a Common Variable, reset the Size to 0., and then restore the Size when the Operation is finished', all by using Macro Variable Formulas.

In fact, if you want to adopt Wear Comp as a standard, you could make your Post output G10 Lines in the header, to clear out all the Geometry Size values, to avoid the issue of an Operator forgetting to clear those values.

I have never been a fan of Full Control Compensation, and feel like any shop who still uses it as a standard, is basically still living in the dark ages. No offense intended...

Thanks for that Colin, I will look into moving over to wear and using G10 to do so . What are the advantages of using wear .

No offense taken I respect your feedback and just want to improve.

Share this post


Link to post
Share on other sites
Just now, megaman said:

Thanks for that Colin, I will look into moving over to wear and using G10 to do so . What are the advantages of using wear .

No offense taken I respect your feedback and just want to improve.

With Wear Compensation, it is much easier for the Operators to see and judge the "amount of change" that is being made.

For example, the Operator runs an Operation to machine a 1.000 Diameter Hole. The Tool they are using, has say, a radius of 0.3714.

When they measure the hole, the diameter they measure is 0.9983.

So, how much change do they need to make in the Compensation Register to adjust the hole diameter?

With Wear Compensation, this is easy to do. The Operator simply enters (-0.0008) into the Wear Register. They could do this with or without using "full control compensation", since the Wear Offset and Geometry Offset data are added together when Comp is applied. (G41/G42, or G41.2/G42.2)  [The -0.0008 is for a machine configured to use Radius values.)

If the Offset Registers were setup to read "diameter values" instead of Radius, then the Tool Diameter would be 0.7428, and the Wear Register would be -0.0017.

I am listing the tool radius/diameter values, to give you an idea of the change needed in the Wear Column. When most shops switch to using Wear Comp, they program using "wear" in the Mastercam Operation, but do not enter the "Geometry Offset".

So the first reason to use Wear Comp, is that is simplifies "making adjustments", because you are directly entering the "change" you want to see. If you use Control Comp, (set to radius for example, then your 0.3714 value, would be changed to 0.3706). So the "adjustment you just made to the 'feature size' is not as easy to detect".

The second reason to use Wear Comp, is this; you can shorten your Lead In/Out moves, where the Comp is applied. (But only if you are not mixing Control and Wear comp.)

For example, if you want to interpolate that 1" hole in our example above, and you have entered -0.0008 Wear Radius Adjustment. The minimum Lead In move required to turn on compensation is only 0.001.

For most finishing Operations, where I'm using Wear Compensation, I use a Perpendicular Line Entry/Exit, of about 0.020, and then use an Arc with about 20-40% "arc sweep angle", to enter/exit the cut. So long as your "lead in/out line" is greater than the amount of Compensation you are applying, it will work without an alarm.

I have used this successfully with Wear to be able to interpolate a hole, were there was only a few thousandths difference between the hole diameter, and the diameter of my tool. (For example, Interpolating a 0.251" Diameter Hole, using a 0.246" Diameter Endmill, and being able to comp the diameter within 0.0001 of true size. My perpendicular entry line was only 0.002, and the amount of Comp I had to apply was about 0.0006. (I programmed the Nominal Tool Diameter of 0.246 in Mastercam). This is extremely difficult to do when using Control Compensation. Most controls will not allow you to do this. With some controls, you can start the tool "above the hole", turn on Control Comp during the lead in move, and then plunge the tool down into the hole, before engaging the cut. You make the cut, then retract the tool out of the hole, before cancelling the Control Comp. It is a pain in the butt, and dangerous to try and get Control Comp to work when your tool size and feature size are very close to the same diameter. With Wear Comp, as long as your 'lead in move' is greater than the 'amount of wear comp' that is being applied, everything just works.

  • Like 1

Share this post


Link to post
Share on other sites

*

*

*

*

By the way, we have a whole thread that is pinned to the top of the Industrial Forum; Compensation Pole, where this is discussed back-and-forth. There is more good information about the differences between the Comp Types in that thread, and is worth reading.

 

Share this post


Link to post
Share on other sites

I'm not sure the standard use of wear comp is available to you in your machines present setup. As Husker said, there is a parameter, on Mazak machines, that allows you to choose between using the actual diameter on the Mazak Tool Data fields for the tool, or using the wear offsets for radius & length in the Tool Offsets fields. Our machines are all setup to use the lengths measured in the Tool Data page & the wear offsets in the Tool Offsets fields.

  • Like 2

Share this post


Link to post
Share on other sites
21 minutes ago, So not a Guru said:

I'm not sure the standard use of wear comp is available to you in your machines present setup. As Husker said, there is a parameter, on Mazak machines, that allows you to choose between using the actual diameter on the Mazak Tool Data fields for the tool, or using the wear offsets for radius & length in the Tool Offsets fields. Our machines are all setup to use the lengths measured in the Tool Data page & the wear offsets in the Tool Offsets fields.

Zeke is exactly correct here. The Parameter Settings on your Control always dictate how your machine is configured. Please consult with your Machine Tool Builder's Application Department for the proper settings for your Machine.

You may run into an issue with this, as most people default to their preferences. They may prefer to use the Mazak Tool page setup, and caution you against making a change. However, I default to "I want to understand and make sense of every available option, so I can help you choose from among the options, the scenario which works best for you".

One of the best things you could do for yourself is to get a copy of the Programming Manual and Parameter Manual for each of your machines. Keep in mind that Parameter Values will also vary, machine-to-machine, based on vintage and installed options.

Share this post


Link to post
Share on other sites
On 2/22/2021 at 11:18 PM, cncappsjames said:

Do you  have a Head/Head machine, Table/Head, or Table/Table machine?

5-Axis drilling isn't technically 5-Axis. It is simultaneous 5-Axis or 4+1 positioning and then drilling along the Z-Axis Vector unless you're using a Right Angle Head. But It should be fine.  All depends on your machine's option package though.

I deal with Table/Table machines and typically my collision checking and post software (CAMplete) does positioning , drilling, canned cycles, etc... using G68.2

I'll have to see what kinds of parts I have and test out what I can get based on the cycle. Hang tight.

I'm sure it's just terminology I'm not familiar with, but what is the difference between these types of machines?  I've seen those terms referenced here a few times, but I'm not sure what is meant by it.

 

Share this post


Link to post
Share on other sites
2 hours ago, JB7280 said:

I'm sure it's just terminology I'm not familiar with, but what is the difference between these types of machines?  I've seen those terms referenced here a few times, but I'm not sure what is meant by it.

 

Head/head is where both rotaries are on the spindle head.

Head/table is where one rotary is on the spindle head and the other is on the table. Also called a hybrid.

Table/table is where both rotaries are on the table. Most common.

Share this post


Link to post
Share on other sites
20 minutes ago, PAnderson said:

Head/head is where both rotaries are on the spindle head.

Head/table is where one rotary is on the spindle head and the other is on the table. Also called a hybrid.

Table/table is where both rotaries are on the table. Most common.

interesting, I don't think I've seen either of those first 2.  Where would something like an Okuma Multus fall?  Would that be Head/Table?

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us