[Martin 007]

High speed pocket feature wasn't doing it..... I posted everything in the basic pocketing feature. Then went in and edited it in Prediter and note pad...
The result came out great... tool marks are smooth.... HSP far left and center are not..... you can feel them.

Thanks for al the help on this ....
Doug

[jrmach]

Always more than one way to do things.in your Cog Thread I hinted I would probably do a different way.Some tool paths do better in certain situations than others.If you would of cut a square out and stuck in vice holding only to the bottom.09,you would now have a situation where you have an open pocket.That is where I would use HSP.The time difference could be up to 2 X as fast.You can really turn up the feed in this situation.When you confine the geometry (using solid lines instead of dashed lines)especially in small sections,HSP In my opinion would not be the best choice.

You mentioned earlier that the code in one place read z-.090 and you said it should of read -.100.I believe in that instance what you where seeing was a re-positioning of the tool with a .010 Floor Clearance.What that means is instead of Retracting all the way back to your Clearance Plane above the part,it is only moving up .010 above the cut to re-position and make another cut.You also have a separate setting for the feed of that.It is a maximum feed instead of a rapid.Hope that clears a little bit up for you.

[Martin 007]

It would seem that the only way I can use the High speed feature woud be it there is no change in the Z axis. Another thing i found was it changing feed rates on every line... This is likely what caused the jerking motions. I think it messes with the controlers slow down feature so not to hit stop from a high speed. It evidenty slows down before the intended change....

Anyway... If it wont add the Z on each line then it wont do me any good... Why the basic can do it and not the HSP... is over my head.

[jrmach]

If you can load the.bbcd file and your PP we can figure it out.Note though HSP would still not be my 1st choice in this particular situation.Did you post code and run the file I gave you thru Preditor?That one works on my end.Anyway we should get to where you can use HSP.In the right situation (and there are many) this is absolutely the tool path strategy of choice to use.Many users agree and many have been bummed it has been not offered since V23.
I was going to upload some information for you that Celertive Technologies (HSP/Volume Mill) use to have on their website.I guess I never saved it and they no longer offer it so their website has no info on it.Maybe someone has some literature on it saved and will share it.You can see what their latest tool path offering is,it is similar in some ways.The more you understand what their strategy is the better you can put it to work for you in the right situatations.FWIW go to your Help Menu/About BobCAD/Celertive Technologies.
As good as I talk about HSP,it does have quirks and sometimes screws up.They all do(at least for me)But the problems you are having I think we can figure out.Like I said a file and PP we can try.

[Martin 007]

Jr. the HSP was suposed to be the answer for my probems with V21. The way it goes about creating the tool path is not the issue its the fact that it's ignoring things. Posting Feed rates higher than my set Max. and biggest issue not posting the Z lines. Anyway here is my basic post which still has a issue or two. Drill stuff not working yet, 4th I havent tried ... all for another day. I wil try and find the instructions... or discriiptions of how and why ... about the control software....
There is tool path for HSP and basic in the program file. and TXT files for each. Inner pocket never changed in both... its basic. I did have to shift the outer pocket to 5/16 for rough because I have no more 1/4 mills. That was for the 3rd attempt... HSP wont even post for that mill. then I finished with a 3/16.
In the middle of some design and Photo work... but will try and get the videos up later....

[jrmach]

"Jr. the HSP was suposed to be the answer for my probems with V21



Are you using V21 or V23????

[Martin 007]

I'm on V23... with BobArt and Updated.... I think the reason they don't offer the HSP (going by what you said) is that they fixed the basic pocket... I have not looked into anything later than 23 so i don't know what they are doing or have... But basic really works a lot better than i remember. Going to push it latter today on some other files... parts that it failed on in V21.
Attached is the command software "" do's and don't's) sorta manual just in case you have a question.... it may be a little off from your basic G-code useage....

[fidia]

I think the high speed toolpaths are ok when you have a machine with very high spindle speed and feedrate like a haas vf2ss. Other than that I wouldnt use them

[SBC Cycle]

Jr. the HSP was suposed to be the answer for my probems with V21. The way it goes about creating the tool path is not the issue its the fact that it's ignoring things. Posting Feed rates higher than my set Max. and biggest issue not posting the Z lines. Anyway here is my basic post which still has a issue or two. Drill stuff not working yet, 4th I havent tried ... all for another day. I wil try and find the instructions... or discriiptions of how and why ... about the control software....
There is tool path for HSP and basic in the program file. and TXT files for each. Inner pocket never changed in both... its basic. I did have to shift the outer pocket to 5/16 for rough because I have no more 1/4 mills. That was for the 3rd attempt... HSP wont even post for that mill. then I finished with a 3/16.
In the middle of some design and Photo work... but will try and get the videos up later....

You aren't getting Z moves because the HSP feature will use helical arcs to sweep into the cut. If you look at Block 64 of your post processor, you will note that there is no z_f called. z_f is a command to output a Z Feed value (that is what you are missing).

64. Arc move XY.
	n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate

I know you have this part figured out already but this will be a recurring problem with HSP until you get that line changed.

[jrmach]

Martin I'll address these questions first

"" I think the reason they don't offer the HSP (going by what you said) is that they fixed the basic pocket... I have not looked into anything later than 23 so i don't know what they are doing or have... But basic really works a lot better than i remember. ""


The way I heard it is Volume mill was wanting a lot more money for their tool path (HSP) and BoB decided it was just too much keep offering it and be competitive.Simple economics.Basic pocketing does not do open pockets so it has absolutely nothing to do with HSP.

In V25 with update 769 BoB came up with a close replacement to HSP,Advanced Pocketing.All that I have used it,it is good.Best of all it is not an add on(doesn't cost extra)

SBC found a problem with PP,that's good.Hopefully that will help a lot.On top of that,what I see as some of the problems with your experience with HSP,is the what your trying to apply it to and how you are trying to apply it.I don't think anyone well disagree with me with the statement that HSP is a very valuable tool in your tool box to have.

Instead of going thru anymore than I have previously,I have some good news,I found the documentation to HSP hiding in a file.I will try uploading it.FYI only the 2axis information sections are pertaining to the HSP you got.Some of the information is slightly different than our version of it,but this should answer a lot for you.

[BurrMan]

You aren't getting Z moves because the HSP feature will use helical arcs to sweep into the cut. If you look at Block 64 of your post processor, you will note that there is no z_f called. z_f is a command to output a Z Feed value (that is what you are missing).

64. Arc move XY.
	n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,feed_rate

I know you have this part figured out already but this will be a recurring problem with HSP until you get that line changed.

[jrmach]

OK,I computed your tool path with HSP the way everything was in your file,and for some reason you are getting an intermediate level of tool path between each level that you imputed in your parameters.


Then I changed your geometry to an open pocket and re-computed without changing a thing,and it computed as it should.

So with the closed pocket something is screwing up big time.Got me.

Burr any thoughts?

[BurrMan]

OK,I computed your tool path with HSP the way everything was in your file,and for some reason you are getting an intermediate level of tool path between each level that you imputed in your parameters.


Then I changed your geometry to an open pocket and re-computed without changing a thing,and it computed as it should.

So with the closed pocket something is screwing up big time.Got me.

Burr any thoughts?

Floor Clearance - The value entered here establishes the Z-component of a helical move that is used when entering or exiting a cut. Only non-negative values are allowed. If a positive value is entered, repositioning moves between cuts will take place above the already-machined floor. If zero is entered, the tool will drag across the already-machined floor during these moves. In this case, set the High Feedrate parameter to be no greater than the cutting feedrate to help ensure more consistent tool marks on the floor

[jrmach]

The level of that intermediary tool path level is approximately .054 which is halfway between levels.His floor clearance is set to .010.Something looks wrong.

[jrmach]

I figured it.I normally use HSP for open pockets so I never encountered this before(at least that I was aware of)

[BurrMan]

My brother used the HSP on a 1/4 hp mill. It made a big difference.

[jrmach]

My brother used the HSP on a 1/4 hp mill. It made a big difference.

[bjm323]

My brother used the HSP on a 1/4 hp mill. It made a big difference.

So the Taig handled the HSP ok?

[BurrMan]

So the Taig handled the HSP ok?

Yes. He was really excited about the improvment in speed and ALSO, just the overall machine stability.

We now use the adaptive roughing of the advanced roughing feature for this. The rounding of the corners and smoothing just makes the machine move like butter, instead of cheddar. AND, the adaptive roughing in the new system respects the "stock selected"... Huge.

[Martin 007]

First off thanks... all of you... I understand what you are talking about... except SBC's find.
1st... BC edited the post and I gave them everything including the command software. The same post for the basic pocket adds the Z value to each Line.. why didn't HSP?

2nd The basic pocket performs the helical ramps smoothly..

With my particular set-up... machine and control software it has however they do it... a Anti-Knock feature so not to rattle the Ball Screws. It ramps the feed rate before the stop or lower feed rate. SP was changing the feed rates on every line. BUT In light of what Jr. found with Z-leval changes... maybe that is what it was doing.

I'm not debating weather or not HSP or Basic is better than the other... They are on the same team as I see it.... But in this case HSP is on the bench... lol Well untill I get it fixed and also learn when and where to use ... well all of them...

I will post the video in a few mins.... it shows the stop and go movements of the HSP It might take me a bit of time to review all of the files you attach and sugestions... Just FYI... Thanks again