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:

Camplete Setup


JB7280
 Share

Recommended Posts

46 minutes ago, JB7280 said:

I'm in FL.  I will try that tonight if I've got time.  I have a part that I got to simulate correctly in Camplete, but I'm using a "tooling ball" location for each rotation offset.  How can I direct Camplete to use that offset?  Even though it posts that way through Mastercam, Camplete seems to handle it differently.

If you are using multiple offsets like g54 55 56 when you go to manage machine, edit I had to set the cam index to 0,1,2 ECT for camplete to respect the work offset. It defaults them all to -1

  • Like 1
Link to comment
Share on other sites
49 minutes ago, JB7280 said:

I'm in FL.  I will try that tonight if I've got time.  I have a part that I got to simulate correctly in Camplete, but I'm using a "tooling ball" location for each rotation offset.  How can I direct Camplete to use that offset?  Even though it posts that way through Mastercam, Camplete seems to handle it differently.

When you use the interface make sure you are using the correct coordinate system for each one of them. If you using extended offsets then that is fine, but make sure you are going through and making sure they are coming in correctly in the CAMplete side of things. If not then you have to change them to what your using.

Link to comment
Share on other sites
33 minutes ago, 5th Axis CGI said:

When you use the interface make sure you are using the correct coordinate system for each one of them. If you using extended offsets then that is fine, but make sure you are going through and making sure they are coming in correctly in the CAMplete side of things. If not then you have to change them to what your using.

Hm, so that's why it gives me P6 when I have 6 for my offset, where MC would normally output P1.

  • Like 1
Link to comment
Share on other sites
41 minutes ago, JB7280 said:

Hm, so that's why it gives me P6 when I have 6 for my offset, where MC would normally output P1.

Yes it does take a little to get use to, but once you do it a few times then it becomes more natural. I changed posts to use 54 for G54 and 55 for G55 and 1 is G54.1 P1 when I worked in shops I programmed in, but since going out and doing it for others I have just stuck whatever a customer is using to make their programs. 

Link to comment
Share on other sites
3 minutes ago, cncappsjames said:

Edit your machine in CAMplete again, on the Coordinate System tab, set G54 as 0, G55 as 1, G56 as 2, etc... and it will behave like a Mastercam Post. 

I liked it when it worked supporting the extended offsets 1 is P1 and so forth. Messes me up trying to go back and remember 0 is 54, 1 is 55 and then 6 is P1. :fish:

  • Haha 1
Link to comment
Share on other sites
5 hours ago, cncappsjames said:

Edit your machine in CAMplete again, on the Coordinate System tab, set G54 as 0, G55 as 1, G56 as 2, etc... and it will behave like a Mastercam Post. 

 

5 hours ago, 5th Axis CGI said:

I liked it when it worked supporting the extended offsets 1 is P1 and so forth. Messes me up trying to go back and remember 0 is 54, 1 is 55 and then 6 is P1. :fish:

Agreed.  I will leave that as is, because it makes more sense.  James, I noticed you had a post FOR Camplete in your z2g file.  Is a different type of post needed for Camplete?  I thought that Camplete didn't care about the post because it did that itself?

Link to comment
Share on other sites
3 hours ago, JB7280 said:

 

Agreed.  I will leave that as is, because it makes more sense.  James, I noticed you had a post FOR Camplete in your z2g file.  Is a different type of post needed for Camplete?  I thought that Camplete didn't care about the post because it did that itself?

The Z2G has what is needed for Mastercam with the MMD, CMD items. I think it was to help you extract them for the Mastercam side of things not for CAMplete. Camplete is the post for your machine.

Link to comment
Share on other sites
4 hours ago, JB7280 said:

 James, I noticed you had a post FOR Camplete in your z2g file.  Is a different type of post needed for Camplete?  I thought that Camplete didn't care about the post because it did that itself?

Correct on all points. The post I created for CAMplete does nothing more than populate text fields. Drill cycle names, High Speed Mode selection through Canned Text, etc. CAMplete would take the data regardless itself it had a name or not. It's just easier to see this way. Look at the drill cycle names... they actually have the G7n/G8n so you know what cycle you're gonna get. Handy, no?

 

That post does NOT generate G-Code. It was never meant to. It was just meant to populate text fields. Make sense?

Link to comment
Share on other sites
3 minutes ago, cncappsjames said:

Correct on all points. The post I created for CAMplete does nothing more than populate text fields. Drill cycle names, High Speed Mode selection through Canned Text, etc. CAMplete would take the data regardless itself it had a name or not. It's just easier to see this way. Look at the drill cycle names... they actually have the G7n/G8n so you know what cycle you're gonna get. Handy, no?

 

That post does NOT generate G-Code. It was never meant to. It was just meant to populate text fields. Make sense?

So it uses the post to populate the misc values fields in the toolpath dialog in MC?  Does Camplete handle the high speed functions without a post like yours?  Sorry for the ignorant questions.  I'm trying to play catch-up, haha.

Link to comment
Share on other sites
36 minutes ago, JB7280 said:

So it uses the post to populate the misc values fields in the toolpath dialog in MC?  Does Camplete handle the high speed functions without a post like yours?  Sorry for the ignorant questions.  I'm trying to play catch-up, haha.

Pretty much. You can set your field names, cycle names. And add the coded thru can text menu.

 

The NC format can be set to output them.

I use the NC format macros and misc integers to set a specific r value.

If there is no override mine will output precision mode for mill or drill mode during drill cycle and 5 axis mode for a multi axis path

 

With the canned text I found it only worked at the beginning of the tool.

 

Link to comment
Share on other sites
45 minutes ago, Leon82 said:

Pretty much. You can set your field names, cycle names. And add the coded thru can text menu.

 

The NC format can be set to output them.

I use the NC format macros and misc integers to set a specific r value.

If there is no override mine will output precision mode for mill or drill mode during drill cycle and 5 axis mode for a multi axis path

 

With the canned text I found it only worked at the beginning of the tool.

 

My NC Format handles the high speed modes for ALL operations, not just first tool. It switches on and off between operations, even operations using the same tool.

I used to use Misc. Int. to handle the High Speed modes but found most programmers didn't apply them or didn;t apply them properly so the function and machine did not perform up to my standard. So, I switched over to Canned Text, created Mastercam Defaults, Default Operations, and Operation libraries with the proper mode set already and now compliance is way up and customers are happier I think. 

R values are the old High Speed Modes. 0 = Canned Cycles/Speed Preference through 10 = Precision Preference.

New High Speed Modes are D, P, M, and F.

G131D1 = Drilling

 

G131P1 = Roughing/General Machining/Speed Preference for 2D/2.5D Cutting Type (think contour pocket, 2D HST, Circle Mill, etc...)

G131P2 = Medium Precision Machining/Balanced Preference for 2D/2.5D Cutting Type

G131P3 = Finish Machining for 2D/2.5D Cutting Type/Precision Preference

 

G131M1 = Roughing/General Machining/Speed Preference for 3D Cutting Type (think surface machining)

G131M2 = Finish Machining for 3D Cutting Type/Balanced Preference

G131M3 = Finish Machining for 3D Cutting Type/Precision Preference

 

G131F1 = Roughing/General Machining/Speed Preference for Rotary Cutting Type (think any rotary type machining)

G131F2 = Finish Machining for Rotary Cutting Type/Balanced Preference

G131F3 = Finish Machining for Rotary Cutting Type/Precision Preference

 

  • Like 2
Link to comment
Share on other sites

I meant a change mid cycle say between tool paths.

Ours turns on and off for tool changes.

If the user does nothing p3 is on. If we want to override a dynamic path we set the integer and real. And set it back at the next toolpath if we want to finish, otherwise p3 comes on at the next tool change.

 

 

 

Link to comment
Share on other sites
1 minute ago, Leon82 said:

I meant a change mid cycle say between tool paths.

Ours turns on and off for tool changes.

If the user does nothing p3 is on. If we want to override a dynamic path we set the integer and real. And set it back at the next toolpath if we want to finish, otherwise p3 comes on at the next tool change.

My NC Formats support between toolpath changes in High Speed Modes.

On mine, if the user does nothing, G131 is output which is equivalent to the old school R8. 

On mine, there is no relationship between the 1st path and subsequent paths... probably because I don't use Misc Int./Misc. Real. I used to use that method. Found it too cumbersome for most programmers to use so we simplified it. 

  • Like 1
Link to comment
Share on other sites
17 minutes ago, cncappsjames said:

My NC Formats support between toolpath changes in High Speed Modes.

On mine, if the user does nothing, G131 is output which is equivalent to the old school R8. 

On mine, there is no relationship between the 1st path and subsequent paths... probably because I don't use Misc Int./Misc. Real. I used to use that method. Found it too cumbersome for most programmers to use so we simplified it. 

I'll have to look at it again. We got ours originally from the matsuura guy and then at times it would stop inserting in mastercam and I had to restart it so I gave up on it

Link to comment
Share on other sites

Where you located @Leon82

My latest NC Format supports High Speed Mode selection through Canned Text, all the coolant modes, Force Tool Changes, TWP, TCP, WSEC, Broken Tool Detection, has the ability to limit Z-Axis full retracts when A/B is at -90. Deg. etc... Lots of goodies. 

In order for things to work correctly, ther's some settings in CAMplete's Mastercam file I/O that need to be set.

PM me for the the settings and NC Format 

  • Like 2
Link to comment
Share on other sites
  • 1 month later...
On 2/19/2020 at 1:29 PM, cncappsjames said:

Where you located @Leon82

My latest NC Format supports High Speed Mode selection through Canned Text, all the coolant modes, Force Tool Changes, TWP, TCP, WSEC, Broken Tool Detection, has the ability to limit Z-Axis full retracts when A/B is at -90. Deg. etc... Lots of goodies. 

In order for things to work correctly, ther's some settings in CAMplete's Mastercam file I/O that need to be set.

PM me for the the settings and NC Format 

I am MOST interested in these tweaks !! 

As well as needing some help...

We have a Matsuura MX520 trunnion and CAMplete. Using X9. (still pushing hard for my company to upgrade !)

I have recently been awarded a new computer (WINDOWS 10).

I have loaded CAMplete on the new box and it seems to be working, for the most part anyway.

However, when I post from Mastercam there seems to be something amiss, as the “Z Rapid” moves are all facing down toward the Z negative direction. Definitely something wrong here…  PLEASE HELP.

I am at a loss, and cannot post through CAMplete for our Matsuura MX520 on my new computer.

 

Going to send a PM as well..

 

Thank you in advance for any assistance you can give me !

Link to comment
Share on other sites

This is what  did. From the start up instructions. It's the third option.

 

1) Start the CAMplete TruePath software

2) Go to Tools > Options

3) Click File Types

4) Select Mastercam and click “Advanced Properties”

5) In “Datum Settings”, enable “Treat WCS Datums As Datum Changes In Same Fixture”

6) Enable “Move Tool Paths To Global WCS And Create Local WCS In Part Coordinates”

7) Enable “Read Datum Index From NCI

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...