HSP: High Speed Pocketing just came out from BobCAD. Has anyone tried the demo yet?

They have a video on their website:

http://bobcad.com/index.php?select_page=mill_standard_full_tabs_page


Screen Shots

http://i564.photobucket.com/albums/ss86/damjuice/1.jpg

http://i564.photobucket.com/albums/ss86/damjuice/2.jpg

http://i564.photobucket.com/albums/ss86/damjuice/3-1.jpg

http://i564.photobucket.com/albums/ss86/damjuice/4-1.jpg

http://i564.photobucket.com/albums/ss86/damjuice/5-1.jpg

http://i564.photobucket.com/albums/ss86/damjuice/6-1.jpg

That's good stuff, I used a similar package in SolidCam.

But what's the story? Is it included in next update or is it to be an additional purchase?

moldmker

If I had to guess its an add on thats not free. but it sure would be a nice upgrade if it was included.
Randy

Looks very interesting indeed. I am however a bit sceptical being that I first got into the V2007 craze just after it came out. With all the trouble with that continuing into V22, I will wait a while to see what problems folks are having before I try it. Those of you that have used V22 and V23, is V23 that much better? Have the issues that V22 experience been ironed out mostly?

Thanks

I would say most if not all the issues with V22 have been addressed or fixed in the V23 software.

I am very happy with the V23 software at this time, but as to be expected there still are a few things that I would like to see changed or addressed.

I did buy the high speed tool path from BobCAD. The salesman started out at $995 for it but I got him down to $495! Which I think is a good deal. I haven't cut any parts with it, and I really don't understand all the options and how to use them yet, but from what I can tell it does what mastercam calls peel milling, 3D ramped slots ( where the tool ramps down the slot to cut it ) Tri cordial pocketing I think is the real name of this type of pocket. Open ended pockets and totally open pockets for very strange bosses. Rough tool, clean up tool, and finish pass tool ( I can't seem to get it to post cutter comp on the finish pass :(

I haven't spent too much time with it but so far it hasn't crashed on any sample I've given it.

The new high speed pocketing is not trochoidal toolpath. Trochoidal tool paths use looping motions in an attempt to avoid burying the tool. This results in a longer toolpath and cycle time. This new HS Pocketing allows constant step-over designed so that the tool will not be buried, except in carefully planned and controlled conditions, thus eliminating the need for circular motion.

Users can define the straight-line toolpath parameters - feed rate, spindle speed, step over and axial depth of cut that offer the best tool life and material removal rate. This HS Pocketing toolpath can then be run safely using those parameters regardless of part geometry or the number of islands. In fact, the resulting paths may look different and possibly can be longer than traditional offset pocketing. However, the V23 HS Pocket toolpath can deliver a faster cycle time by maintaining the heftiest cutting parameters possible throughout the cut.

Sincerely,
CNC Dude

Just so everyone out there knows, you will have a new build to update to probably tomorrow. This will have some fixes and enhancements outside of the new HS Pocketing. Release notes will be made available to customers. You can now project curves to surfaces on user defined coordinate systems, general posting things, drilling operation tweaks, UCS correction when there are multiple shapes on a UCS other than the top, the system was calculating toolpaths in the wrong location. That has been corrected. A few other items have been cleaned up as well.

I'll tell you, we've come a long way and the results are really good.

Stay tuned!

CNC Dude

I'll tell you, we've come a long way and the results are really good.

Stay tuned!

CNC Dude

Yes I will say Bobcad has come a long way from V2007

Thanks for the information everyone.

CNCDude, I have a few questions concerning this new toolpath. How will this work on older machines?

This is my situation. I have a Mazak VQC-20/40B. It has a Mazatrol (Mitsubishi) CAM M-2 control. This machine is vintage 1983-84. It has some limitations, first being memory (I have 24K to work with), second becuase it is an early M2 control it doesn't have "Tape Mode" so no drip feed is possible(firmware upgrades aren't cheap), third being an older control doesn't have very good block look ahead and processing speed (maybe 3 or 4 blocks).

On several jobs, the memory and processing capability become major issues for me. I end up breaking down the programs between tools and running each tool seperatly on each part. Also with Z-Level rough, going around arcs bcc breaks it down into many small linear increments, this causes my machine to stall and dull the tool. After about 4 parts the tool has dulled to the point it starts to chip. If I'm lucky I can get 12 parts before the tool is completely gone. So about every 12 parts I am up for a $60 endmill.

With this in mind will the H.S. toolpath work for me? Does the program break down the movements into linear segments or does it do arcs? When compared back to back on the same part will the program length be more or less on the HS vs. the regular Z-Level rough. Also, is this basically just a 2D toolpath at this point, or can it be used similar to the Z-Level rough? One part I make is a pocket with tapered sides and 2 islands. It's the one that gives me the headaches mentioned above.

Yes, I know I need a newer machine. Right now I want to get by with what I have before upgrading to something newer due to the economy, I'm sure everyone here can understand that. If V23 w/ HS machining will help me out it would be worth it.

Thanks

nlh,

There is an option in the Z-Level Rough to convert the movements into arc segments. On teh posting page there is an Arc Fit option. Click the button so that it is depressed, and then compute and post the toolpath. You may want to play with the Tolerance, to get more or less arcs, but the option is there.

The HS Pocketing is a 2-2.5D operation in its' current state, so it can't be used with solid geometry. You need to instead use wire frame. If you can pocket this part that you are talkinbg about, and then follow through with a Z-Level finish, then yes, this toolpath operation would be of benefit to you.

Regards

Hi NLH,
I have 2 Leadwells' with the MO control, which I think are less advanced than the M2. Mine do not run like that unless I am really running them with programs that have tiny steps(.0005")

It almost sounds like you may be running in exact stop mode, if your machine stutters running from internal memory.You could try running in high speed mode, this smooths the toolpath and might help.

I like the sound of the new High speed machining, I have been waiting for V23 to get a bit more de-bugged and it seems like it is getting there.

Regards,
Cutmore

Cut More,

Thanks for the information. I will have to look into the exact stop mode. Would this be a G or M code, or possibly a parameter?

The One,

Maybe Arc Fit is all I need for that particular part. The machine has no problem running the equidistant path on the same part.

Concerning the H.S. toolpath, how does it break down the program, into arcs or linear segments? Will this toolpath require high HP and heavy rigid machines?

Thanks

Sorry I missed your question nlh. Looks like the One covered it. Has anyone looked at the demo or seen the video on the BobCAD-CAM website?

CNC Dude

Hi NLH,
the high speed mode is a g code, G05 P01,G05 P02,
G05 P0 cancels the mode.

I haven't used it yet, but maybe it will help you.


Hope that helps,
Cutmore

Thanks Cut More,

I'll give it a go maybe tomorrow if I get a chance. Although I'm not entirely sure the Meldas M2 and Mazatrol M2, even though both built by Mitsu, are the same beast. I do know that I have "3D Option Roms" installed. The machine came that way when I got it, but no one, even Mazak, has been able to tell me how to use them or what they do. The joys of having ancient iron. I'm hoping the G05 is what the roms are for.

Thanks again

BTW, What is the difference between P1 and P2 in G05?

Hi NLH,
I posted a screenshot of the page in the programming manual about the high speed mode.

THe difference seems to be that in highspeed p1 you can use tool diameter offset, and the speed is limited to 16.8m/min.

In highspeed p2 you can not use the diameter offset, and the speed is limited to 67m/min.

If I could machine anything at 16m/min I would be astonished!

You can download the programming manual from the mitsubishi site if you do not already have it BTW.

Regards,
Cutmore

Cutmore,

No luck with my machine. It's just too old. The 3D Roms are for the mazatrol which I don't use anyway. Had a quick look in my manual and came across a G64 continouos cutting mode, buy it appears the machine is in that mode when I turn it on anyway. Put it in a program and saw no difference. Still stops momentarily after a move. Most noticeable when transitioning from G3/G2 to a G1. Thanks though, you just never know until you try.

Sorry to hijack the thread.

Hi everyone i bought it today make sure you haggle for it they will come down a long way.I purchased it seperatly i aleady have pro mill and predater upgrade v23 has been working great since i upgraded from v22 .I hope this will do away with the excevive moves in pocketing all that wasted time i have anouther sys and it does about half the moves to do the same thing i am hoping this will speed things up a bit.I am running most feeds about 15ipm and i hope to pick it up quite abit and hope the accuracy stays the same we will see not sure of the spindle speeds though that maybe my limiting factor.

If you would like to try some sample code, you can go to http://www.celeritive.com/index.php. They have a 14 day free trial where you can upload a dxf file, and produce code that you can then run on your machine. I will be trying it either tomorrow or Sunday. I want to see how it works on my older machine. FYI, this is the code that v23 uses for it's HS pocketing.

Can anyone tell me why this would happen . You can not change the posting unless you are in the editor.

Found out they wrote the software and started selling it but did not update the post prossesors for them which they seem to think is the problem and I have not recieved one yet but will let yall know.

You don't need to wait for BobCAD to update the post. You can actually get the code output to work for the HS Pocketing with a simple edit.

Open the Post Processor file in Notepad.
Look for line 64 in the post, there may be two so look at the bottom of the file in case.
Change the line so that it says: g_arc_plane, g_arc_move, x_f, y_f, z_f, arc_center, feed


That should get you the output you are after. The only thing you need to have attention on is getting that z_f in there right after the y_f. Use a comma to separate the variables though.

Regards

You don't need to wait for BobCAD to update the post. You can actually get the code output to work for the HS Pocketing with a simple edit.

Open the Post Processor file in Notepad.
Look for line 64 in the post, there may be two so look at the bottom of the file in case.
Change the line so that it says: g_arc_plane, g_arc_move, x_f, y_f, z_f, arc_center, feed


That should get you the output you are after. The only thing you need to have attention on is getting that z_f in there right after the y_f. Use a comma to separate the variables though.

Regards

Hi The One
Can you tell me if this change should be done to all post processers or was it just for the one posted? I'm running Mach 3 Metric.

If your line 64 does not have the z_f variable in the line then it should definitely be added. If your using a custom post processor, one you have already modified, then you will want to download the post from the web and use a diff tool to see what the differences are.

There are some additional lines in the posts for the recent release, build 1326. They pertain, mainly, to the header needed for the Predator Editor to do a backplot.

Regards

If your line 64 does not have the z_f variable in the line then it should definitely be added. If your using a custom post processor, one you have already modified, then you will want to download the post from the web and use a diff tool to see what the differences are.

There are some additional lines in the posts for the recent release, build 1326. They pertain, mainly, to the header needed for the Predator Editor to do a backplot.

Regards

Thanks The One
I had not modified my post and I had download build 1326. My post didn't have the z_f part in it. The post processsors on the support site also didn't have it.
So my post line 64 now looks like
64. Arc move.
n,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate

Should I also add in g_arc_plane?
Or better yet - where could I download the standard Mach 3 Metric Post for High speed pocketing?

Those posts should have all been updated. Do you have the automatic tool changer? I can post it here for you.

I have talked to Brain at Mach3 and the post that I have on my system is approved for the machines without the ATC.

Regards

Those posts should have all been updated. Do you have the automatic tool changer? I can post it here for you.

I have talked to Brain at Mach3 and the post that I have on my system is approved for the machines without the ATC.

Regards

Hi
That would be great if I could post it here for me. I don't have the ATC.
Regards

Just make sure you are getting x,y&z in a g02 or g03 move because that was my problem . If not it will drop into the material instead of feeding into it .
I want to say that my post was cleaned up and everything seems to be fine.
The response was very quick as i do believe it was just foresite.
The tool path is great if you have a high spindle speed and can handle light cuts at super fast feeds . We are running at 300 ipm. but it does not always run that though. Which makes my cutting time down to at least half.
The only thing is if i pick two hole ops. and tell them one is 54 and one 55
it makes them both what ever the fist one is . So im going to have someone look at this. I am running on haas machines also . so if you would like this post vfmill.mlpt please reply.

I recently purchased the HSP package. I am having trouble getting the circular moves to also drop in z. The path looks good in Predator. If I post the code I get only z moves in the straight line moves.

I played around with the post using the recommendations somewhere else on this post. It didn't seem to help.

Am I missing something?

Anybody else using the HSP?

Thanks,

Robert

open your post in the note pad and look at line 64.
This is what it should look like.
64. Arc move.
n,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate


once you do this just click on file and then click on the save button ,not the save as button.

Laserkey,

I tried editing the post. I was carefull to cut an paste exactly as you have shown. Still, in predator the path looks good. The post however doesn't show Z movement in circular paths.

I made a tech request to Bobcad for assistance.

Otherwise the path seems to work well. The movements are full arcs instead of broken line segments. Should cut very fast.

I'll let the forum know as soon as I have some real pockets to cut.

Robert

Robert,

Based on my limited experience (V23 demo, and volumill's 14 day website trial), the material entry is not a true helical path. More of a rectange, picture the cutter moving in a linear path, then performing a 180deg. arc, a linear path in the opposite direction and then another 180. The z moves should be in the linear portions, not the arcs. Which is why it looks like it's working correctly in predator, but examination of the code makes one think otherwise. It took me a little bit to catch this one myself. Hope this helps.

Nate

Robert,

More than likely, there is more than one line 64 in your post. This is a case of "the last one wins". Look at the very bottom of the post in a text editor. You should see an additional line down there that needs to be changed or removed. I would suggest removing it if it is there and if you have already modified the line 64 that is in the right location.

Regards

Thanks everyone,

There were two line 64's. After editing the second one HSP does spiral down in the G03 lines and continues at the same rate in the G01 lines. This way the descent angle doesn't violate the ramp rate the endmill is capable of.

I am anxious to practice on some pockets and compare cycle times and endmill life.

As nlh suggested, the ramp is sort of a rectangle. But, I get G03 x,y,z and G01 x,y,z drops. This is the way I understood the path to work.

I'll post some paths and reviews as soon as I can.

Thanks again,

Robert

Glad to hear you have it working Rob,

Will be interested to hear how it works out when cutting material. Keep us posted. BTW, what machine (make, model, control) will you be using?

Nate

nlh,

I work several jobs. Primarily I am plant engineering, using mostly Mori Sieki mills and lathes with Fanuc 0 and 10 controls. The part time shop has a variety of machines. Ranging from older Mazaks to latest with Fanuc 21i. I mostly program the fanuc based machines with subs and macros. They have me come in for these 'special needs' programs using macro variables, adjusting the cutter comp path sequentially as we jig grind, etc.

This HSP will save me a lot of work.

I've read the forum for years, I am going to try to be more proactive when people need help. I see a large variety of problems/solutions.

Thanks again,

Robert