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:

Rookie Mistake


Corey Hampshire
 Share

Recommended Posts

A little context to start. I do a lot of 4th axis mill programming. Rotary on the table. I do a lot of 3+1 and some Multi-Axis also. 

Last week I made a rookie mistake. I import most of my operations and on this particular part I had to use a different tool path. I forgot to change my WCS back to Top on one operation and smoked a milling cutter. Everything looked good in Mastercam as the rotary position is obviously driven by the post processor.

How can I keep this from happening in the future? Some parts I get over 100 operations on and it's very easy to miss the fact that one of my WCS is incorrect. I do not have any simulation software that is driven off my g-code. I'm working on the boss to move that way, but in the mean time I would like to come up with a work around. 

Is there a c-hook or does anyone have a slick way to select all ops and make sure all WCS are set to Top plane when posting out? I'm sure that I'm not the first guy that has done this, and I won't be the last! 😂

Any one got any suggestions to keep this from happening in the future?

Link to comment
Share on other sites
7 minutes ago, htm01 said:

if you use X+ for a set up sheet you can have it list WCS name, even if you don't use the sheet you could run it as a check

THIS PLUS 10X BILLTRILLION!!!

It is 1x click so fast and easy - you can have it output Coolant, Work offset numbers, H + D to ensure they match etc etc.

So fast and a great double check.

  • Like 2
Link to comment
Share on other sites

I always use X+ for set ups and just for the notes also, since when you bounce around on multiple machines and then things sit for a while you can get back in sync with the jobs just by reviewing the X+ notes that you made and your ready to go . 

+ GAZILLION TO Gunther !!!

I  and Others Thank Gunther For The Fine Work That He created For us all to use.

:cheers:

  • Like 6
Link to comment
Share on other sites

I downloaded X+ and I have to say I am impressed! It is very nice to run a report and see things laid out in a simple quick check. I also discovered the work offset button, that will save me some messing around as well. Not that it is a big deal to use edit selected operations, but the fewer mouse clicks the better. I setup hot keys for these tasks so they really are one button for me.

Is there a place to add notes on the setup sheet as mentioned above? I don't see it, but am probably over looking it.

Thanks for the suggestion on this, I will definitely be using this in the future! 

  • Like 1
Link to comment
Share on other sites

There's a pretty simple way to do this without using any add-ins, unless I'm missing something about your question:

  1. Click on your machine group to select all operations
  2. Right click in the toolpath manager
  3. Select "Edit selected operations" then "Edit common parameters"
  4. Click the check-box next to planes and set your planes

 

Link to comment
Share on other sites
13 minutes ago, JHyder2 said:

There's a pretty simple way to do this without using any add-ins, unless I'm missing something about your question:

  1. Click on your machine group to select all operations
  2. Right click in the toolpath manager
  3. Select "Edit selected operations" then "Edit common parameters"
  4. Click the check-box next to planes and set your planes

 

I need my C Plane and T Plane to stay what they are set at per operation. If I use the method you suggested I cannot keep them separate. Hopefully in the future Mastercam will give us the option to edit just the WCS, TPlane, or CPlane individually. Thanks for the suggestion though!

  • Like 1
Link to comment
Share on other sites
1 hour ago, Corey Hampshire said:

I need my C Plane and T Plane to stay what they are set at per operation. If I use the method you suggested I cannot keep them separate. Hopefully in the future Mastercam will give us the option to edit just the WCS, TPlane, or CPlane individually. Thanks for the suggestion though!

Yes, this is a royal PITA, when you need to change the WCS, but want the T/C Plane Combinations to remain the same.

The best way I have found is to do this:

  • Set your WCS, Cplane and Tplane, to a given "rotation" plane. (one you want to "correct")
  • Select "All Operations" in the Toolpaths Manager
  • Right-Click in the Ops Manager, and use the "Select" function in the RMB Menu
  • In the "Select" dialog box, there is an option to select Operations by "Plane". This should be the Active Toolplane, for a given set of Operations. For example: if you have 200+ ops, but Operations 53, 55, 105, 111, and 187 all use "B330. - Angled Port Holes" for the Toolplane, then you will see that "plane name" in the drop-down list. Mastercam in this case, will report "5 Operations Found".
  • Now, press the Green Check Mark.
  • When the dialog closes, those Operations will be "Selected" with the Green Check Mark.
  • Now, use "Edit Selected Operations > Edit Common Parameters", and it will change only the Ops that have the matching T/C Plane Combo. So when you do a "Planes", it will copy the current WCS, Cplane and Tplane into the dialog.

This prevents you from changing any Ops that you don't want too...

  • Like 8
Link to comment
Share on other sites
30 minutes ago, Colin Gilchrist said:

Yes, this is a royal PITA, when you need to change the WCS, but want the T/C Plane Combinations to remain the same.

The best way I have found is to do this:

  • Set your WCS, Cplane and Tplane, to a given "rotation" plane. (one you want to "correct")
  • Select "All Operations" in the Toolpaths Manager
  • Right-Click in the Ops Manager, and use the "Select" function in the RMB Menu
  • In the "Select" dialog box, there is an option to select Operations by "Plane". This should be the Active Toolplane, for a given set of Operations. For example: if you have 200+ ops, but Operations 53, 55, 105, 111, and 187 all use "B330. - Angled Port Holes" for the Toolplane, then you will see that "plane name" in the drop-down list. Mastercam in this case, will report "5 Operations Found".
  • Now, press the Green Check Mark.
  • When the dialog closes, those Operations will be "Selected" with the Green Check Mark.
  • Now, use "Edit Selected Operations > Edit Common Parameters", and it will change only the Ops that have the matching T/C Plane Combo. So when you do a "Planes", it will copy the current WCS, Cplane and Tplane into the dialog.

This prevents you from changing any Ops that you don't want too...

Pretty much how I do it as well.

  • Like 1
Link to comment
Share on other sites

I would say that a demand that all the WCSs in an NC-program are identical is a pretty universal demand. So why not make your post check that all your WCSs are the same as the 

one  specified in the first operation ? That takes you out of the check loop.  I have been doing that now for many years.   

Gracjan 

  • Like 1
Link to comment
Share on other sites
3 hours ago, pullo said:

I would say that a demand that all the WCSs in an NC-program are identical is a pretty universal demand. So why not make your post check that all your WCSs are the same as the 

one  specified in the first operation ? That takes you out of the check loop.  I have been doing that now for many years.   

Gracjan 

Buttttt..... (granted that i'm rusty now....) if you want to machine a simple 3ax 2op part...

OP1 (Vice) WCS#1 G54

M00 (FLIP)

OP2 (Fixture) WCS#2 G55

M30

?

  • Thanks 1
Link to comment
Share on other sites

 

In the case  you  presented you could have the built in warning system of checking the WCS , but since you know  that  it's OK, you get warned by the post , but post it out anyway knowing all is fine in THIS CASE .

it*s the 50 ops where one is  programmed with a different WCS than all the rest that will overwhelm You ,  that's where my WCS check would be worthwhile ...

 

Gracjan

  • Like 4
Link to comment
Share on other sites
16 hours ago, Colin Gilchrist said:

Yes, this is a royal PITA, when you need to change the WCS, but want the T/C Plane Combinations to remain the same.

The best way I have found is to do this:

  • Set your WCS, Cplane and Tplane, to a given "rotation" plane. (one you want to "correct")
  • Select "All Operations" in the Toolpaths Manager
  • Right-Click in the Ops Manager, and use the "Select" function in the RMB Menu
  • In the "Select" dialog box, there is an option to select Operations by "Plane". This should be the Active Toolplane, for a given set of Operations. For example: if you have 200+ ops, but Operations 53, 55, 105, 111, and 187 all use "B330. - Angled Port Holes" for the Toolplane, then you will see that "plane name" in the drop-down list. Mastercam in this case, will report "5 Operations Found".
  • Now, press the Green Check Mark.
  • When the dialog closes, those Operations will be "Selected" with the Green Check Mark.
  • Now, use "Edit Selected Operations > Edit Common Parameters", and it will change only the Ops that have the matching T/C Plane Combo. So when you do a "Planes", it will copy the current WCS, Cplane and Tplane into the dialog.

This prevents you from changing any Ops that you don't want too...

Thanks Colin. I have never used the selected option off the RMB before today. I see there are other options to use too. it's always great to learn new things like this!

  • Like 1
Link to comment
Share on other sites
3 hours ago, pullo said:

 

In the case  you  presented you could have the built in warning system of checking the WCS , but since you know  that  it's OK, you get warned by the post , but post it out anyway knowing all is fine in THIS CASE .

it*s the 50 ops where one is  programmed with a different WCS than all the rest that will overwhelm You ,  that's where my WCS check would be worthwhile ...

 

Gracjan

Thanks for the suggestion. I think I will get with my reseller and see about having them add a warning to the post. We only use this machine for 4th axis work so there really shouldn't be any instances where the warning would be a bad thing. That said, could I have it set up to toggle the warning being active with a Misc value? I honestly know nothing about the posts, it's all over my head.

Link to comment
Share on other sites

#variable definitions
swcs_name : ""   #PRM20014
swcs_name1 : ""
swcs_name2 : ""  # to check if there are different WCS's , they should all be the same

fq 53  swcs_name2 "OOPS , rogue  WCS in your program!!!! "

pparameter$    # Initialize variables, and Run parameter table
         
         if prmcode$ = 20014 , swcs_name = sparameter$  #WCS name

pheader$


        swcs_name1 = ucase(swcs_name)  

ptlchg0$     # Null tool change 
        
         swcs_name2 = ucase(swcs_name)
         if swcs_name2 <> swcs_name1 , q53

ptlchg$
         swcs_name2 = ucase(swcs_name)
         if swcs_name2 <> swcs_name1 , q53

 

very basic stuff for anybody who dabbles in posts

Gracjan

  • Like 1
  • Huh? 1
Link to comment
Share on other sites
14 minutes ago, pullo said:

#variable definitions
swcs_name : ""   #PRM20014
swcs_name1 : ""
swcs_name2 : ""  # to check if there are different WCS's , they should all be the same

fq 53  swcs_name2 "OOPS , rogue  WCS in your program!!!! "

pparameter$    # Initialize variables, and Run parameter table
         
         if prmcode$ = 20014 , swcs_name = sparameter$  #WCS name

pheader$


        swcs_name1 = ucase(swcs_name)  

ptlchg0$     # Null tool change 
        
         swcs_name2 = ucase(swcs_name)
         if swcs_name2 <> swcs_name1 , q53

ptlchg$
         swcs_name2 = ucase(swcs_name)
         if swcs_name2 <> swcs_name1 , q53

 

very basic stuff for anybody who dabbles in posts

Gracjan

I am constantly amazed at the knowledge on this forum. This is over my head. Maybe one day I can aspire to know how to modify posts. Thank you for this info.

Link to comment
Share on other sites
2 hours ago, Corey Hampshire said:

Thanks Colin. I have never used the selected option off the RMB before today. I see there are other options to use too. it's always great to learn new things like this!

The "Select" function from the Right Mouse Button (RMB) Menu is a slick tool to be aware of.

I use it all the time for figuring out 'which geometry' is tied to a particular operation, or which operations use a 'given tool'. You can even search by 'string', which will search through the Operation Comments for a given 'snippet' of comment.

  • Thanks 1
  • Like 1
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...