Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Hosed myself on WCS plane, hopefully for the last time


nperry
 Share

Recommended Posts

Was doing a simple 4X mill job the other day (part had been outside the shop for a while for centerless grind and gun drill, note: no setup pieces because we tried to drill these ourselves in house and it didn't go well) and I totally hosed myself on WCS plane. Created a new plane for A235., the WCS went to that plane instead of A0., naturally, and I didn't catch it, because I was under the gun with a bunch of stuff and in a hurry. So the hole that was supposed to go in at A235. went in at A0. instead. Luckily the customer is still buying the part, so we dodged a bullet there, but the point remains...

I've been burned on not catching an incorrect WCS plane a few times now, and mostly it results in hurt pride. That one was bad because it was only 10 operations...on some of these jobs where I'm doing multiple hundred operations I can forgive myself a bit for it, but not in this case.

So, being that I'm mostly only outputting from one WCS at a time, am I missing some sort of trick for locking that one specific plane in as my WCS? I was thinking about adding a message to the post that would holler at me when I'm outputting more than one WCS at a time, if that's possible.

Link to comment
Share on other sites

To me, that's just part of being a programmer.

Better than 75% of what I program is HMC work, generally with hundreds of OP's and a ton of transforms..for me, it's just the habit.

I tried setting up  something via the post, I found it was more of a problem than the one it was supposed to solve. I do rely on Machsim to help too.

M2C. the guy in the seat needs to pay attention to what he's doing, check, double check and triple check if need be..

 

  • Like 1
Link to comment
Share on other sites

I ran X+ setsheet for this. 

One click and it would output all the ops in order, with Speed Feed, T# H+D, Coolant, and G54/55etc.

Literally 30 seconds of scanning, and you can see if all your datums are correct, and that H+D match T number, you haven't forgotten coolant etc etc

Link to comment
Share on other sites
12 minutes ago, JParis said:

To me, that's just part of being a programmer.

Better than 75% of what I program is HMC work, generally with hundreds of OP's and a ton of transforms..for me, it's just the habit.

I tried setting up  something via the post, I found it was more of a problem than the one it was supposed to solve. I do rely on Machsim to help too.

M2C. the guy in the seat needs to pay attention to what he's doing, check, double check and triple check if need be..

 

Fully agree with you.

I'll still take a little extra idiot-proofing if I can find it, however.

10 minutes ago, Newbeeee™ said:

I ran X+ setsheet for this. 

One click and it would output all the ops in order, with Speed Feed, T# H+D, Coolant, and G54/55etc.

Literally 30 seconds of scanning, and you can see if all your datums are correct, and that H+D match T number, you haven't forgotten coolant etc etc

This could work really well...thanks for the idea!

  • Like 3
Link to comment
Share on other sites

Get a locked WCS put in the post if you use only one WCS at a time. 

With the addition of Automatic Planes things with WCS went in the wrong direction in my opinion. There is no logic or thought to that process. Here is the help section on it.

Quote

Select Automatic to automatically assign a matching work offset number (if one exists), or the next available number if no matching work offset number is found.

Okay so when you come back to the same face why would the system make a new offset number? Why are we still using 0 for 54 in 2021? 

My rule of thumb assign the workoffset in the planes manager before making any toolpaths. As I make new planes make sure I assign the work offset, but when I miss it trouble is coming. 

  • Like 2
Link to comment
Share on other sites
1 hour ago, Greg_J said:

Every time I post a program, Every time. I search for G55, G56, G57, G58 and G59 in Cimco. 

That's how I catch my mistakes.

It didn't output a new work offset. I duplicated my A0. plane and rotated it to A235., so it kept the G54 offset. It was set as my WCS for that operation though so instead of outputting A235. it output A0.

Link to comment
Share on other sites

Maybe something that can help....

I output all of my offsets into my post like this...it can be a quick visual reference to see all of your angles

 

With my HMC work I ONLY output G54.1 offsets...so a rogue G54 would output separately and be instantly visual

(****PLATE 1****) 
(G54.1P1 - B90. - PART - 01)
(X0 +.1668 FROM CENTER OF C'BORE)
(Y0 -1.8042 FROM CENTER OF C'BORE)
(Z0 +.298 FROM FACE OF RAIL)
G90G10L20P1X-7.8315Y-5.1277Z-27.9148
 
 
(G54.1P2 - B90. - PART - 02)
(X0 +.1668 FROM CENTER OF C'BORE)
(Y0 -6.5542 FROM CENTER OF C'BORE)
(Z0 +.298 FROM FACE OF RAIL)
G90G10L20P2X-7.8315Y-9.8777Z-27.9148
 
 
(G54.1P3 - B90. - PART - 03)
(X0 +.1668 FROM CENTER OF C'BORE)
(Y0 -11.3042 FROM CENTER OF C'BORE)
(Z0 +.298 FROM FACE OF RAIL)
G90G10L20P3X-7.8315Y-14.6277Z-27.9148
 
 
(G54.1P4 - B90. - PART - 04)
(X0 +.1668 FROM CENTER OF C'BORE)
(Y0 -16.0542 FROM CENTER OF C'BORE)
(Z0 +.298 FROM FACE OF RAIL)
G90G10L20P4X-7.8315Y-19.3777Z-27.9148
 
 
(G54.1P5 - B270. - PART - 01)
(X0 -.1668 FROM CENTER OF C'BORE)
(Y0 -1.8042 FROM CENTER OF C'BORE)
(Z0 -.025 FROM TOP OF STOCK)
G90G10L20P5X7.8315Y-5.1277Z-27.7182
 
 
(G54.1P6 - B270. - PART - 02)
(X0 -.1668 FROM CENTER OF C'BORE)
(Y0 -6.5542 FROM CENTER OF C'BORE)
(Z0 -.025 FROM TOP OF STOCK)
G90G10L20P6X7.8315Y-9.8777Z-27.7182
 
 
(G54.1P7 - B270. - PART - 03)
(X0 -.1668 FROM CENTER OF C'BORE)
(Y0 -11.3042 FROM CENTER OF C'BORE)
(Z0 -.025 FROM TOP OF STOCK)
G90G10L20P7X7.8315Y-14.6277Z-27.7182
 
 
(G54.1P8 - B270. - PART - 04)
(X0 -.1668 FROM CENTER OF C'BORE)
(Y0 -16.0542 FROM CENTER OF C'BORE)
(Z0 -.025 FROM TOP OF STOCK)
G90G10L20P8X7.8315Y-19.3777Z-27.7182

Link to comment
Share on other sites

crrl,alt,shift,p held at same time and I pick whatever post I want. This way I have seperate posts locked to g54 g55 ect. Especially on rotary work with transform/rotate use. 

Personally I think it should default to locked and prompt me if I want multiple work offsets. I also believe the entire model should come in as a check surface and you grab what you want to cut. I don't think you should have to worry about running a raster toolpath and having to fight vialating other surfaces  or make a bunch of boundary curves to keep cutter from rolling into surfaces you don't want to  machine. Start everything out safe and click a box a box if you want to get risky. Not start all in risky with planes and work offsets and not model aware and have to manually tie them all down. jmo

Link to comment
Share on other sites
On 8/28/2020 at 8:45 AM, nperry said:

It didn't output a new work offset. I duplicated my A0. plane and rotated it to A235., so it kept the G54 offset. It was set as my WCS for that operation though so instead of outputting A235. it output A0.

I always name my main WCS such as OP1 or OP2 and in the planes lock page, input 0 to lock it as G54. Before I post any toolpaths, visually scan each toolpath path and look for WCS: “Name of Main WCS Plane”. you can be 100% confident it’ll post the right angle position and work offset

Link to comment
Share on other sites

This is how I attempt to prevent this issue. Unfortunately the 'Change common parameters' won't work for this, because there is no option to change "only the WCS Plane". If you use Common Parameters, then it will override the Plane selection as well.

What I do is Right-click in the Ops Manager, and choose the 'Display options'.

This function allows you to choose what information is displayed in the Ops manager.

I turn everything "off", except for WCS Name. This turns off all the other display information, so only the WCS Name is displayed in your Ops Manager. You can now scan through 100's of Operations quite easily, since all the "visual clutter" has been hidden.

Once you have scanned through the Ops list, and made any corrections, go back to the display options and turn on the Op Comments, T/C Plane info, and all the other display options.

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
On 8/28/2020 at 9:07 PM, So not a Guru said:
On 8/28/2020 at 10:08 AM, Greg_J said:

Every time I post a program, Every time. I search for G55, G56, G57, G58 and G59 in Cimco. 

That's how I catch my mistakes.

Yep, it only took being bit a couple of times before this became a habit.

This kept happening in our system last year, 

we use a c# application to parse the nc file and create a setup sheet, it throws an error if g55 g56 g57 g58 or g59 are found.

You could write a script to do that with this nethook, the wcs thing could be checked with a chook, I do have a project that does this.

Link to comment
Share on other sites
On 8/28/2020 at 6:03 AM, nperry said:

Was doing a simple 4X mill job the other day (part had been outside the shop for a while for centerless grind and gun drill, note: no setup pieces because we tried to drill these ourselves in house and it didn't go well) and I totally hosed myself on WCS plane. Created a new plane for A235., the WCS went to that plane instead of A0., naturally, and I didn't catch it, because I was under the gun with a bunch of stuff and in a hurry. So the hole that was supposed to go in at A235. went in at A0. instead. Luckily the customer is still buying the part, so we dodged a bullet there, but the point remains...

I've been burned on not catching an incorrect WCS plane a few times now, and mostly it results in hurt pride. That one was bad because it was only 10 operations...on some of these jobs where I'm doing multiple hundred operations I can forgive myself a bit for it, but not in this case.

So, being that I'm mostly only outputting from one WCS at a time, am I missing some sort of trick for locking that one specific plane in as my WCS? I was thinking about adding a message to the post that would holler at me when I'm outputting more than one WCS at a time, if that's possible.

The "trick" I use is to use a template for Mastercam that has WCS defaults assigned for every viewsheet. Every operation has it's own viewsheet template. Most people do not like viewsheets but I find them to be one of the best parts of Mastercam.

Link to comment
Share on other sites
On 8/30/2020 at 7:39 AM, Colin Gilchrist said:

This is how I attempt to prevent this issue. Unfortunately the 'Change common parameters' won't work for this, because there is no option to change "only the WCS Plane". If you use Common Parameters, then it will override the Plane selection as well.

What I do is Right-click in the Ops Manager, and choose the 'Display options'.

This function allows you to choose what information is displayed in the Ops manager.

I turn everything "off", except for WCS Name. This turns off all the other display information, so only the WCS Name is displayed in your Ops Manager. You can now scan through 100's of Operations quite easily, since all the "visual clutter" has been hidden.

Once you have scanned through the Ops list, and made any corrections, go back to the display options and turn on the Op Comments, T/C Plane info, and all the other display options.

This is how I teach doing that sanity check as well.

Link to comment
Share on other sites

Ideally Mastercam would have a native function that would query the operations and graphically display the number of wcs's/cplanes/tplanes used in a selected group of operations inside of the viewport.

That's just personal preference, but I would rather draw information as text in the viewport so that the user has the option to print it.

Link to comment
Share on other sites
3 hours ago, byte said:

Ideally Mastercam would have a native function that would query the operations and graphically display the number of wcs's/cplanes/tplanes used in a selected group of operations inside of the viewport.

That's just personal preference, but I would rather draw information as text in the viewport so that the user has the option to print it.

Adding to your thoughts is to expand on that the automatics workoffsets would be kinematically aware. You would see the work offset for the Plane when shown as part of the display options. It would also tied back to the control and machine definition to show that which the post would be using. Why I will name mine G54 Zero or G55 Zero for Fanucs. H1 Zero or H2 Zero for Okuma and etc... depending on the machine. Jim Varco added that support to his Active Reports to change what active reports shows depending on your machine. As the Mayor calls it scorched earth so I struck it out. Mastercam in the world of Machining stuck in a rut with certain things because of the 30 years of we have always done it this way and the core code that ties so much of what was done 30 years ago to the current classes and other things related to the heart of the software. GROUP is one thing that comes to mind. 0=54 for workoffset outputting, C and T planes for Toolpaths. The 99% of users never need these functionalities, but it is the core of the software and since they have to try to keep over 200,000 legal users and 1,000,000 illegal users of Mastercam using it they do what they can to keep them all happy. 

  • Like 1
Link to comment
Share on other sites
On 8/28/2020 at 7:03 AM, nperry said:

So, being that I'm mostly only outputting from one WCS at a time, am I missing some sort of trick for locking that one specific plane in as my WCS? I was thinking about adding a message to the post that would holler at me when I'm outputting more than one WCS at a time, if that's possible.

Here is a tiny chook that will graphically diplay text with the number of active WCS in the file excluding manual entries.

The ft function is called "Get Property -> num Wcs"

propertyManager-AddIn.zip

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...