Sign in to follow this  
Joe777

CAmplete TruePath

Recommended Posts

I'm just curious, was anyone able to correct an issue with Camplete-completely ignoring "Manual Entry" from Mastercam.

Dear Jesus! If you can hear me.

 

Share this post


Link to post
Share on other sites

You need a format macro with a custom gcode label

 

So when you type a manually entry it should look like this in master cam

 

ME1,M00

ME2,( change clamp)

Some NC  formats have it in there otherwise you might have to add it.

 

So if camplete sees me1, in the NCI it outputs it as unsimulated code

On our NC format it's located in the start path block

Share this post


Link to post
Share on other sites

I also have a couple other macros (mt1, mb1,) to insert it in specific points before and after a tool change once you figure it out it's easy to work with

I have a separate machine definition with probing cycles in the drill paths. The post I changed to output the mb1, instead of block numbers. So from manual entry you choose pick a text file and pick the program. And it's seamlessly inserted to complete. Now we don't need subs for probing cycles.

 

Currently it supports 500 lines of code. But when I'm bored and have time I add more and more it's just slightly labor-intensive on the camplete side to add the g-code label lines

Share this post


Link to post
Share on other sites

Leo, Please pardon my ignorance. I understand what you mean by ME1 and ME2 labels and I know where " start path block " is.  I just can't figure out the correct NC Format.

Thanks.

Share this post


Link to post
Share on other sites

I can post some screenshots of my macros tomorrow if you want.

 

If you have active maintenance they would probably do it for free for you I believe.I sent them some things on my personal email once I don't know if they ever charge us for it or not. The boss never said anything to me so I'm assuming It was free

Share this post


Link to post
Share on other sites
2 minutes ago, Leon82 said:

I can post some screenshots of my macros tomorrow if you want.

 

If you have active maintenance they would probably do it for free for you I believe

Next time I'm to see Mr.Katsu: I'll will personally ask him about Simens Cublex-42 frankenstein!

Share this post


Link to post
Share on other sites

m131.thumb.png.1d830f4670dd687f4ac5a8dae8aa314e.png

Excuse my frustration, but I have trouble any of these to get working. All I get is M131 without any further output, the finish looks like after chewed  up splines.

Share this post


Link to post
Share on other sites

All of those will insert the respective macro when the misc real it set to that value. It looks like that's setting the g131 values

 

The manual entry will be similar, I don't remember the exact parameter name off the top of my head

  • Thanks 1

Share this post


Link to post
Share on other sites

I ran out of space here so I uploaded them to an image hosting place

 

https://postimg.cc/gallery/9M2MTn4

So you basically have to make a macro called MANUAL_ENTRY with the custom gcode dialog.

 

There is one box to add a new line up at the top and at the bottom there's a box that says add codes.

So insert like 10 lines and copy the example

  • Like 3

Share this post


Link to post
Share on other sites

You'll also need to set in the Options Advanced Settings the "Post Insert Custom GCode As Comment" as unchecked. By default it is checked. 

Share this post


Link to post
Share on other sites

You could use Canned Text instead of Misc. Int./Misc. Reals as well. I think it's a cleaner method.

image.png.141440ed1c0b0362db60489e43be83bb.png

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites

In your manual entries @Joe777, they will need to be formatted as follows, set to "as code", and EXACTLY as you want to see it;

ME1,M00(REMOVE 1ST CLAMP)

ME2,(TORQUE TO 10Nm)

ME3,M00(DID YOU DO IT?)

ME4,M00(ARE YOU SURE?)

 

As @Leon82 stated, in this case the "ME1,", "ME2,", "ME3,", etc... is the flae CAMplete sees which tells it to output the string of text and needs to be put in places you may want to see a manual entry output like before tool changes, after tool changes, between operatinos that use the same tool, end of program, etc... It needs the comma as well. No comma, no output.

Share this post


Link to post
Share on other sites
On 7/9/2020 at 10:34 PM, Leon82 said:

All of those will insert the respective macro when the misc real it set to that value. It looks like that's setting the g131 values

 

The manual entry will be similar, I don't remember the exact parameter name off the top of my head

From our Hypermill post, not related to Camplete:  It seems to be HONRx .

Hopefully it helps someone:  on mam72-35 fanuc it's standard G131 P,M,F. On our's mam72-63 fanuc it's G131 R.  On Cublex-42 siemens 840 it's HONRx.

Share this post


Link to post
Share on other sites
19 minutes ago, Joe777 said:

From our Hypermill post, not related to Camplete:  It seems to be HONRx .

Hon for Siemens g131 for fanuc. as you read it into fanuc it will strip the h on and replace it with G 131.

So Fanuc doesn't like O's in their programs other than at the top. My coworker spent a half an hour swearing at his USB stick. But he put an MO in that had an XO instead of x0

Share this post


Link to post
Share on other sites
26 minutes ago, Leon82 said:

Hon for Siemens g131 for fanuc. as you read it into fanuc it will strip the h on and replace it with G 131.

So Fanuc doesn't like O's in their programs other than at the top. My coworker spent a half an hour swearing at his USB stick. But he put an MO in that had an XO instead of x0

Leo, could you please shed some light on Cycle832? It's like Cycle800 and Traori  was not enough. Seems to be zero reference to 832 in Camplete. Yet, it indirectly mentions HONRx.

Share this post


Link to post
Share on other sites
8 minutes ago, Joe777 said:

Leo, could you please shed some light on Cycle832? It's like Cycle800 and Traori  was not enough. Seems to be zero reference to 832 in Camplete. Yet, it indirectly mentions HONRx.

I don't have experience with it. Our old es800 3 axis use hon. The j300 yasnak uses GON.

 

All of our mx machines are fanuc

Share this post


Link to post
Share on other sites
17 hours ago, Joe777 said:

Leo, could you please shed some light on Cycle832? It's like Cycle800 and Traori  was not enough. Seems to be zero reference to 832 in Camplete. Yet, it indirectly mentions HONRx.

CYCLE832 is a method to specify vector tolerances. It's probably not explicitly supported though it probably could be;

	TRAORI
	ORIAXES
	ORIWKS
	CYCLE832(0.005,_ORIFINISH,0.05)
	ORISON
	..........
	ORISOF
	

ORISON = Orientation Smoothing ON which activates the smoothing of the orientation vectors.

ORISOF= Orientation Smoothing OFF which deactivates the smoothing of the orientation vectors.

The ORI tolerance should be set to the CAM tolerance * sqrt³ *10


The ORISON function can only be used in conjunction with 5-axis transformations TRAORI. It's not part of CYCLE832 or CUST_832 and needs to be programmed separately in the workpiece program if vector smoothing is required.

  • Like 1

Share this post


Link to post
Share on other sites
18 hours ago, Joe777 said:

From our Hypermill post, not related to Camplete:  It seems to be HONRx .

Hopefully it helps someone:  on mam72-35 fanuc it's standard G131 P,M,F. On our's mam72-63 fanuc it's G131 R.  On Cublex-42 siemens 840 it's HONRx.

To further clarify, HON Rx is the old style High Speed Modes. You have R0 through R10. R0 for canned cycles when profile tolerance is of no concern, R1 for roughing through R10 for Fine Finishing. I believe the CUBLEX Series (FANUC), MAM72-63V and the Siemens controlled machines are the last machines that use this.

HON P,M,F,D are the new high speed modes that are tuned for specific toolpath types. P = Prismatic Type Machining. Contour, Pocket, Circle Mill, Engraving, Helix Bore, etc.... M = Multi-Surface Machining, F = Rotary type toolpaths, and D = Canned Cycle toolpaths. Each mode has 3 programmable settings (HONP1, HONP2, HONP3, HONM1, HONM2, HONM3, HONF1, HONF2, HONF3) with the exception of D. If using D, D=1 always.  Within each setting P/M/F, 1 and 2 have 3 adjustable settings via the sliders on the MACH LEV. screen. These can;t be set by program yet. I've put in the request. P/M/F 3 has 4 adjustable settings. The MX Series (MX-330, MX-520, and MX-850), MAM72-35V, MAM72-70V, and MAM72-100H use this method for high speed modes.

If a program contains HON... and is read into the control via a FANUC function the control converts HON to G131. If the program is transferred via FTP, no such conversion takes place and the program will be riddled with errors. This is the reason we have defaulted CAMplete to have G131instead of HON. FAR less support calls.

The Siemens is a completely different beast. It follows the old HON Rx method. It's been a while since I've put my hands on one, but I believe no conversion is necessary.

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
Sign in to follow this  

  • 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