X5 tool paths with arc filter twice the size in x5 as x4

[neurosis]

Has anyone else been noticing that the posted g-code is double in size of what was coming out of X4? I have a part file that I pulled in to X5. I have the arc filter set exactly the same using all of the exact same cutting parameters. The X4 file posts at 300K. The X5 file posts at 660K. This particular part has several splines used to create a cam profile. These are all 2d dynamic tool paths. The programs are so big that they will no longer fit in to our control. The original posted program size was 389k for the entire program. The X5 posted g-code is over 800k for the exact same part with no modifications! WTH!

 

Edited to add that the 2d spline/contour paths, the filter changed itself when the part file was changed from x4 to x5. I have the contour paths tamed down and are now the same size as in X4. The dynamic tool paths however, I cant adjust the filters enough to bring the size down to even close to what they were in X4 without bringing the filter tolerance over what the wall offset is.

[gcode]

Go to the Mastercam App in the Control Panel

Click on the "Toolpath Support " page

By switching the drop down from X4 to X5,

you can compare the settings betwee X4 and X5 and

see if anything is set differently

[neurosis]

Everything looks the same. I looked in the config as well to see if I had the same settings in there and they are. The only place that I am noticing this is with the dynamic milling paths so far (along with some strange things that go on when i open old files in X5. things seem to like to change themselves for some reason). Every single one of my 2d dynamic tool paths in this file have the same arc filter settings and the x5 file version of the paths are 2 to 3 times the size.

[gcode]

did you check the sliders at the top of the filter page..

they seem to default to Longest and Best in X5

[neurosis]

These are 2d dynamic paths. I dont believe that there is a slider.

 

One thing that I am noticing though. The linear movements do not show up in back plot. They only seem to post as linear movements. One of the 2d dynamic paths are a pocket that is helicial ramping in to. In X4 the helical entry posts as arcs. In X5 it linearized the entry but only during posting. It does not show up during back plot. It shows it as an arc movement. it seems to be linearizing quite a few of the xy arcs as well. They show up in backplot as arcs but post as linear movements.

[gcode]

did you check to make sure your X5 control def (arcs page) is supporting helix motion.

I've had a lot of trouble with the arcs page reseting itself to default settings during post upgrades

 

 

edit.. I just tried a 2D dymanic I did last week..

It posted helix (arc) entry with 2 different posts... so I'd look at your control def..

[neurosis]

The control def "is" set up supporting helical motion. and as i said, the 3d arcs are not the only issue. it is linearizing the 2d arcs as well. I had this issue in X4 at some point as well with 2d contours and some arcs. I wonder if it is the same problem. I cant remember what the cure was.... it was a tolerance settings somewhere.

[gcode]

use the CD Compare Chook to compare

your X4 and X5 Control Defs

[neurosis]

The chook only allows me to compare two x5 control defs.

[gcode]

The chook only allows me to compare two x5 control defs.

 

you're right.. I was sure I've used it to compare an X4 and X5 control def...

must have been during the beta cycle... sure can't do it now

 

If you've got dual monitors, you can put an X4 and X5 control def side by side and compare them

the only pages you really need to compare are the tolerance and arc pages

[neurosis]

I just shrunk the windows down and put them side by side on my monitor. The two are identical from x5 and x4. I re-generated the op and was able to get it to helical interpolate. circle mill also helical interpolates just fine. I still cant figure out why two exact same dynamic milling tool paths, one in X5 and one is X4, with the same parameters and arc filter settings, are posting as much as 3X more code... ug!

 

Tomorrow I am going to create a similar shaped geometry flat pattern. I'll start with a fresh X5 file and create the same path with the same parameters. I'll do the same in X4. I'll compare the two and see what the results are.

 

What is confuses me, is that I can see when I run the path in back plot, it is creating arcs in X5. they are just posting as segments.

[neurosis]

Ok, I started from scratch here using the exact same geometry pulled in to two "NEW" part files it both X4 and X5.

 

I used the exact same settings for everything including the arc filter. I used one of the default X5 machine definitions rather than a imported X4 just in case.

 

The tool path in X5 is more than double the size! 256K in X4 and 564K in X5. That is pretty significant. Am I the only one seeing this? Or seeing it as an issue?

[gcode]

just out of curiosity, post the nci from both files and compare their sizes.

If they are of similar size, I'd suspect a post problem.

 

If the X5 NCI is way bigger than the X4 NCI its an X5 problem

I find this disturbing as many of the machines I work with have tiny memory

and this has the potential to cause me all sorts of grief.

Whatever the cause it needs to be adressed.

email me your X4 file

I'll post it in X4 then import to X5 and see what I get... and I'll send it to qc if need be

[neurosis]

just out of curiosity, post the nci from both files and compare their sizes.

If they are of similar size, I'd suspect a post problem.

 

If the X5 NCI is way bigger than the X4 NCI its an X5 problem

I find this disturbing as many of the machines I work with have tiny memory

and this has the potential to cause me all sorts of grief.

Whatever the cause it needs to be adressed.

email me your X4 file

I'll post it in X4 then import to X5 and see what I get... and I'll send it to qc if need be

 

 

Thanks Gcode! I will work on it tomorrow!

 

I am working at home right now on my laptop having to view mastercam through vnc so it is very hard to see what in the xxxx I am doing.

 

I used default machine def and post files in both X4 and X5 when I created this earlier today. I will see what I can do about getting you "both" files and you can see what you find out.

 

This is very disturbing to me as well as I use dynamic roughing on almost "every" file that I work on now. I didnt realize how much I have grown to depend on it until I noticed this little issue. I am hoping that it is me that is doing something wrong here.

[gcode]

I just did a simple 2d dynamic area mill in X4

I posted it with X4 then imported the file into X5

the posted fies from X4 and X5 were identical

[gcode]

Tried the same thing with a 2d core mill with very small step overs to get a decent file size

The X4 and X5 NC files were NOT identical, but they were the same size

I'm using the stock 3X VMC post

[neurosis]

Tried the same thing with a 2d core mill with very small step overs to get a decent file size

The X4 and X5 NC files were NOT identical, but they were the same size

I'm using the stock 3X VMC post

 

 

I couldnt wait... Do you want to see if you can make heads or tails of this? Obviously the one with the X5 extension is the x5 file. The X5 file reads 600k for this operation.. the X4 file reads 246k. please tell me what I am missing. The difference is in the NCI file.

[gcode]

Very weird..

I didn't even open your parameter pages

I opened each file, regened and posted

the X4 NCI is 173K

the X5 NCI is 250K

 

 

the X4 NC file was 101K

the X5 NC file was 108K

 

this machine is my laptop which hardly ever gets used

so both installs are pretty much stock

I did notice that the X4 is X4 MU2 not MU3

 

try this... open your X5 settings/config

go to the Files page

in the right window scroll down to Mill Postproccessor.exe

click on the file cabinet and check the path and version of mp.dll

make sure this is your X5 install folder.. not an X4 ( or X3) folder

It should look something like this

 

C:\Program Files (x86)\mcamx5\apps\MP.dll

 

I'm showing mp.dll version 14.0.4.33.

 

If its not your X5 install look at my siggy and see if it applies

Your config file may be jacked up.

Close X5 then move ( or delete) your config file

Launch X5.. a new config file with correct paths will be generated

[neurosis]

Not only did I not copy any files over the top of the X5 install, I did not import any configs from x4. I set everything up in X5 from stock. The only path that I modified during the install was the drive that X5 was installed on... Drive D rather than C. Other than that X5 was a complete stock install. I did import my machine def files and posts but the part files that I created here were both created is stock X4 (for x4 file) and X5 (for x5 file) machine def's.

 

The mp.dll is showing the correct location and version.

 

To be clear with you on sizes that I am talking about (600k vs 250k) I am looking at the sizes shown in the operations manager. I didnt post either one of these files nor did I post the nci.. I was giving you the sizes shown in the operations manager only. There is a huge difference in size between the two mastercam versions. The files that I uploaded are very stripped down versions of the original part file. The original part file contains about 7 dynamic roughing operations for different areas of the part. The differences between x4 and x5 for this "original" part file after posting are enough that the program will no longer fit in the control of our machine. Something is obviously different.

[Tyler Robertson]

I couldnt wait... Do you want to see if you can make heads or tails of this? Obviously the one with the X5 extension is the x5 file. The X5 file reads 600k for this operation.. the X4 file reads 246k. please tell me what I am missing. The difference is in the NCI file.

 

I'm getting the same thing as you - looking at it more. also takes longer to post

[neurosis]

I'm getting the same thing as you - looking at it more. also takes longer to post

 

 

Yes! What I notice when I dig in to the nc code, is that it does not match what is showing in back plot. In allot of areas, the back plot shows the tool path in arcs yet it posts in segments. This makes even less sense to me when trying to figure out what is going on. I turned display points on in backplot and the two files look identical (as far as i can tell). I dont understand why the operations manager would show such a huge difference in size between the two versions.

 

If I post the IGES file only would someone care to re-create the path on their computer and see if they get the same results if nothing else, to prove to myself that it is not something that I am doing here?

[Richard Thomas - Mastercam UK]

Neurosis,

 

I downloaded your files and I have noticed that in a few places X5 breaks straight line moves into smaller segments than in X4 (seen in Backplot). Even with the filtering switched off the NC code in X5 is 2000 lines longer than the NC from X4 (32000 lines vs 30000 lines)

[gcode]

I'm showing the 600K vrs 250K difference in the OP's manager but only a couple of K difference in posted code

if you shut the filter off and regen, both files report similar sizes in the OP's Manager NCI.

The difference is in the filtering routine.

Maybe they built some safety checks in that result in a larger NCI in the OPs manager??

I'm not seeing a huge difference in posted NC code. the difference is 7K in this example, using a stock generic mill

post.

[neurosis]

I'm showing the 600K vrs 250K difference in the OP's manager but only a couple of K difference in posted code

if you shut the filter off and regen, both files report similar sizes in the OP's Manager NCI.

The difference is in the filtering routine.

Maybe they built some safety checks in that result in a larger NCI in the OPs manager??

I'm not seeing a huge difference in posted NC code. the difference is 7K in this example, using a stock generic mill

post.

 

 

In my original file, which contains several of these roughing operations... even with the arc filter adjusted, I am seeing a 200k difference in posted code size. I understand that in some machines this may not be significant, but in some of our machines, this will be the difference between being able to use this tool and not. Something has obviously changed. I wonder what it was and why. And if it will be changed back.

 

I talked to CNC a long time ago regarding 2d core with the z arc lead ins and how much extra code that it created. Again, some of our machines have very little memory.. 128k in fact.. I told them that the amount of code that came form those extra movements made the path useless to me due to our memory limitations... they basically gave me the attitude that we need machines with more memory rather than they need to produce less code. My point in saying that is that this worries me. If this attitude carries over then this could very well become another tool that I lose.

[Guest]

In my original file, which contains several of these roughing operations... even with the arc filter adjusted, I am seeing a 200k difference in posted code size. I understand that in some machines this may not be significant, but in some of our machines, this will be the difference between being able to use this tool and not. Something has obviously changed. I wonder what it was and why. And if it will be changed back.

 

I talked to CNC a long time ago regarding 2d core with the z arc lead ins and how much extra code that it created. Again, some of our machines have very little memory.. 128k in fact.. I told them that the amount of code that came form those extra movements made the path useless to me due to our memory limitations... they basically gave me the attitude that we need machines with more memory rather than they need to produce less code. My point in saying that is that this worries me. If this attitude carries over then this could very well become another tool that I lose.

 

In today's day and age, that is an out dated machine, now I understand that is the tool you have. Perhaps it's time to consider a DNC. That would alleviate any memory limitations that you have and allow you to use ALL of the tools available to you.

 

JM2C