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:

Some camplete tricks i worked on


Recommended Posts

1. using a machine parameter to alter output.

we have 4 types in our shop.

mx330.mx520,mx520pc4 and an mx850. we want the program to end differently for all 4.

edit the machine and create a parameter. Its not showing here but apply to machining setup.

so each machine will have a different number

1.png

make a format macro how you want it to end.

330 goes to g53x-11. 850 and 520 go to tool change position in x pc4 calls m98p1 pallet program

label them so you know what they do

2.png

you can see here i used the same parameter to call a save index macro also

3.png

call them up in the end program block

4.png

here we can call them up in other areas

 

5.png

  • Like 1
Link to comment
Share on other sites
5 hours ago, Tim Johnson said:

Does anyone use Camplete for Nakamura mill turns? If so is it worth the purchase?

I have used it on several different machines. Which model do you have? Mastercam has started offering them in MT environment and not tested any of them yet, but with the addition of Lower/Upper Model support for Part and Steady rest in 2021 that was huge. Send me a PM and we can talk about it. 

Link to comment
Share on other sites
2 minutes ago, crazy^millman said:

I have used it on several different machines. Which model do you have? Mastercam has started offering them in MT environment and not tested any of them yet, but with the addition of Lower/Upper Model support for Part and Steady rest in 2021 that was huge. Send me a PM and we can talk about it. 

We are getting quotes from several manufacturers for a mill turn. The Nakamura rep was showing our director Camplete and I was asked about it. I'm sure we'll get Vericut for whatever machine we get. With that said is there still redeemable value with Camplete along with Vericut?

Link to comment
Share on other sites
2 minutes ago, Tim Johnson said:

We are getting quotes from several manufacturers for a mill turn. The Nakamura rep was showing our director Camplete and I was asked about it. I'm sure we'll get Vericut for whatever machine we get. With that said is there still redeemable value with Camplete along with Vericut?

CAMplete has the Sync Manager and allows you to post the NC code form it. Building tooling in CAMplete is doable by the end user though their main person for the Mill/Turns will fight you tooth and nail to do them all for you. Great guy and has good information on his website for supporting the machines, but he is only one guys supporting all the Mill/Turns for Methods if Methods is your local dealer. The group at CAMplete are a great group always willing to help. Vericut is only simulation and you will have purchase a Post for it and SYNC multi Channels in your head. It will be a lot of trail and error getting the syncing down making sure it works correctly if you're new to it. If you have Multi Channel machines now and just adding a new one to the mix then you understand. If not then CAMplete is a good tool for seeing all the syncing and being able to adjust things in the CAV environment without needing to spend as much time on the machine doing it. That said I feel on Multi Channel machines the last 5% of syncing to get the best cycle time reductions are done at and in front of the machine by an experienced person knowing what to look for.  

  • Like 1
Link to comment
Share on other sites

some manual entry work.

you can change where it outputs. we currently have 3, in the path me1, before the tool change mb1, or after tool change mt1,

7.png

here is one where i modified the post processor to output formated for camplete

probe cycles. those custom names act weird if you are not in the active group

0.png

post

3.png

select as text file

1.png

post from camplete your probe cycles, no manual edits needed

4.png

manual entry macro calls placed in the tool change block

5.png

mb1, macro with 500 lines usable code length

6.png

 

 

these are the tool break calls from the first post

INSERT-MACRO-ENDMILL.png

  • Like 1
Link to comment
Share on other sites

Nice work @Leon82

Many ways to skin the cat with CAMplete. It's the reason I use it for all my posting. Even 3-Axis, and yes for technically unsupported machines. :DIt's a POWERFUL tool.

I personally don't see any reason to use Vericut since I have all of Matsuura's machine configurations; B, A/B, A/C, B/C  (4-Axis HMC, 5-Axis HMC, 5-Axis VMC respectively). Not everyone has that luxury.

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

Nice work @Leon82

Many ways to skin the cat with CAMplete. It's the reason I use it for all my posting. Even 3-Axis, and yes for technically unsupported machines. :DIt's a POWERFUL tool.

I personally don't see any reason to use Vericut since I have all of Matsuura's machine configurations; B, A/B, A/C, B/C  (4-Axis HMC, 5-Axis HMC, 5-Axis VMC respectively). Not everyone has that luxury

 

Thanks, I've actually done that for some three-axis stuff too. It's a nice double check

  • Like 1
Link to comment
Share on other sites

I've been migrating away from using Misc. Int/Reals for a while. We had some complaints from new programmers that there was insufficient detail in the Misc. Int/Real field to describe the function often times. So, we migrated high speed modes over to Canned Text (20-30);

image.png.8dd57e9473ef0bea15e782228380189b.png

image.png.f455a5d69ded8d290cf928208ff84155.png

Customers liked this. Most were still using Misc. Int/Reals for tool breakage though. Recently a few customers have asked to have the ability to measure a tool at the beginning (immediately following tool change) as well as check for a broken tool. So we migrated them over to the Canned Text Method for that as well (Canned Text 11 and 12). There's lots of areas in the machine's configuration that I can exploit as well.

image.png.d6465a47015165cb33441b8164ddbf9a.png

image.png.7fa09fe7788464edf681a940938b6038.png

image.png.b08028da3387600abe5ee55fc754b8f5.png

image.png.260a259fc285117982ab842375f38af2.png

 

image.png.abaca09e5af145a9bdbcc264a228784d.png

I like the WYSIWYG factor in CAMplete. I'm fully capable of doing all this in a Mastercam post but it's more involved. As they say in business, time is money... when I can do all this AND have it tested and collision checked in a matter of minutes instead of hours or days... that's a win in my book especially considering the large variety of machine tool configurations I support.

 

Thanks again @Leon82. You gave me a few ideas.

  • Like 4
Link to comment
Share on other sites

My personal preference on things like tool break checking...

I do them as a manual entry. If they are turned on by something like a Misc Int then you have to expand and open the operation to see if you have it on or not.

As a manual entry, it is right there, you can see at a glance if you have it on a tool or not. I also do them with a custom G code...much easier to remember especially if you are using a Renishaw one place and a Marpos or Blum or whatever on a different machine. For our set up, G103 is always a tool break check.

 

 

Screen Shot 042.JPG

  • Like 2
Link to comment
Share on other sites
37 minutes ago, MIL-TFP-41 said:

My personal preference on things like tool break checking...

I do them as a manual entry. If they are turned on by something like a Misc Int then you have to expand and open the operation to see if you have it on or not.

As a manual entry, it is right there, you can see at a glance if you have it on a tool or not. I also do them with a custom G code...much easier to remember especially if you are using a Renishaw one place and a Marpos or Blum or whatever on a different machine. For our set up, G103 is always a tool break check.

 

 

Screen Shot 042.JPG

When I tried to use the the g-code remap we have it ended up too many levels deep and tried to tool change before it was in the atc position. It alarmed out

2 hours ago, cncappsjames said:

I've been migrating away from using Misc. Int/Reals for a while. We had some complaints from new programmers that there was insufficient detail in the Misc. Int/Real field to describe the function often times. So, we migrated high speed modes over to Canned Text (20-30);

image.png.8dd57e9473ef0bea15e782228380189b.png

image.png.f455a5d69ded8d290cf928208ff84155.png

Customers liked this. Most were still using Misc. Int/Reals for tool breakage though. Recently a few customers have asked to have the ability to measure a tool at the beginning (immediately following tool change) as well as check for a broken tool. So we migrated them over to the Canned Text Method for that as well (Canned Text 11 and 12). There's lots of areas in the machine's configuration that I can exploit as well

I like the WYSIWYG factor in CAMplete. I'm fully capable of doing all this in a Mastercam post but it's more involved. As they say in business, time is money... when I can do all this AND have it tested and collision checked in a matter of minutes instead of hours or days... that's a win in my book especially considering the large variety of machine tool configurations I support.

 

Thanks again @Leon82. You gave me a few ideas.

Our format had the canned high speed mapping as well. One version in mastercam was buggy with adding and removing it so I had changed it.

  • Like 1
Link to comment
Share on other sites
  • 1 year later...

MAM tailstock simulation

The can be done in the macros or machine cycles. I did these in the macro because camplete was crashing when I was editing the cycle. I will touch on this later.

move the base position

base1.jpg

extend the tailstock

base1.jpg

call the macro, in this case from a misc integer

mac1.jpg

delete the mcode from the controller settings because it is a manual base. when you trigger the tail stock it will simulate but not post the mcode.

mcode.jpg

retract it when your done.

I don't retract the base position because it doesnt move.  you could put it in the program start block if you wanted

ret.jpg

ret2.jpg

I you aren't using the 3+1 block you should check the box and copy the 3+2 block into it. this will allow you to keep it engaged during c axis rotations at b-90. I also changed it to only unclamp c axis to save a half a second during indexes.

here you see it is out.

show.jpg

 

If your tailstock_main has no underscore camplete will crash if you try this in the machine cycle. camplete emailed me a new option file.

name.jpg

same principal for the laser. we dont use an mcode so i deleted it from the controller mcodes. it will still simulate it, just wont spit out the mcode.

Screenshot-2021-10-16-065126.jpg

 

  • 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...