Surface High Speed (titanium)?

[neurosis]

Using X2 MR2, is the surface high speed consistent enough to attempt to high speed machine titanium? Ive tried everything playing around and there are a couple of areas, particularly in the first passes, where it buries over 50% of the tool even though I tell it that I only want a max of 10%. This would shatter the tool. I also cant get it to stop ramping from 1/2 " above the part. I have the z clearance set to 0 and in the Linking parameters, I have the Clearance plane set to 3" and the part clearance set to .1. When it starts the helical entry it wants to start at 1/2 " above the part.

 

I cannot put this part on the ftp unfortunately. The picture below shows one of the first passes that buries close to 50% of the cutter.

 

[pip]

Under the helical entry box, is a parameter to change that z start distance, I think

[neurosis]

[Steve Hattori]

Neurosis, I have successfully used HSM for 6-4ti, but it was programmed with Cimco's Adaptive clearing software. Removed 40 lbs of ti with a 3/4 em, .75doc, .03 radial engagement, 400 sfm,, 60 ipm feed. The Cimco sofware allows you to control the engagement exactly, and the cutter lasted 140 mins at this rate. You can try it out for a month for free...Cimcohsm dot com

[neurosis]

I was kind of hoping that I wouldnt have to use 3rd party software to get this working. I am a little apprehensive to try this in titanium as it is. Aluminum would be fine im sure.

 

I saw a video on High Speed Machining Titanium programmed with Surfcam Velocity. That was what gave me the idea to try it. Their tool path looks very good and I cant seem to get the same results out of Mastercam unfortunately. Not blaming the software here, I just dont use the HSS tool path much and I either cant find the correct combination of settings, or the software just is not capable of doing what I am wanting it to do.

 

Is there much difference in the surface high speed machining tool path in X3 MU1 vs X2 MR2? Maybe X4 will produce acceptable results?

[Ocean Lacky™]

One workaround ( there's that "W" word again) would be to increase your stock size by an amount equal to the radius of your tool. It will give you some air cuts, tho.

[Tyler Robertson]

Check your Steep Shallow settings and then your stepdowns - do you have "add extra cuts" elected? The helix could be coming from your Minimum depth being set above the clearance plane

[Steve Hattori]

AFAIK, MC does not have any toolpath that controls engagement the way Surfcam or Cimco does...I bought Cimco's HSM several years ago because I was tired of breaking tools and having to stand there crank the feed knob all the time..

There was a guy on here a while back with a product like that, but I can't remember the name.

[neurosis]

quote:

---

Check your Steep Shallow settings and then your stepdowns - do you have "add extra cuts" elected? The helix could be coming from your Minimum depth being set above the clearance plane

---

The minimum depth is set to the top of the part. I suppose that there is no reason that it needs to be the top of the part. Its actually set to 1.45 where the top of the part is 1.5 so the minimum depth is actually .05 down from the top of the part.

 

I do not have "Add Cuts" checked.

 

 

quote:

---

AFAIK, MC does not have any toolpath that controls engagement the way Surfcam or Cimco does...I bought Cimco's HSM several years ago because I was tired of breaking tools and having to stand there crank the feed knob all the time..

---

That is not good to hear. If you cannot control the engagement any better than this then it makes the High Speed machining pretty much useless for anything other than aluminum or even in some situations in aluminum as well. "Most" of the path generated looks "OK" but there are some areas that just flat would not work. I would be looking at a broken tool. I looked for any examples on the net that I could find of Mastercam High Speed Machining anything other than aluminum in a similar situation and came up empty.

 

quote:

---

One workaround ( there's that "W" word again) would be to increase your stock size by an amount equal to the radius of your tool. It will give you some air cuts, tho.

---

That is exactly what I ended up doing but my stepovers are .05 so it adds "several" air cuts in the areas that did not need modified. I may try to play with the geometry a little and just add a tab in the trouble area and see what happens. I dont understand why this would be an issue. There is obviously a problem where the maximum tool engagement is concerned and how matercam is interpreting it.

 

I placed a surface under the stock geometry and added it to the drive surfaces hoping that mastercam would see it as part of the machinable part but it didnt make any difference. It still engages close to 50% of the cutter even though I told it that I wanted a maximum step over of .0625.

[Chris Rizzo]

Can you strip all the proprietary stuff out of this file and share it?

[cobra95kev]

You simply can't get a Surfcam Tru-Mill type path out of Mastercam. Tru-Mill is simply awesome for hard or abrasive metals. It increases tool life by almost double and cuts faster. Your best hope for now with mastercam is the adaptive clearing that was mentioned earlier. I have played with both and adaptive clearing is alot closer to Surfcam but still not quite there.

 

If you are on current maintenance and can wait for X4 to do it I think it is going to have a tru-mill style path. I can't think of the name of it right now though. I think it might be dynamic mill?

 

BTW: in that large cutout on the top of your picture you could draw some 2D geo and use peel mill and get a decent result.

[Jayson Kramer]

(You simply can't get a Surfcam Tru-Mill type path out of Mastercam.) Not true but you need X4 for this.

 

(Maybe X4 will produce acceptable results?) I am thinking so.

 

But the HSM from Cimco is really nice I am playing with this in X4 now.

[YoDoug®]

+10000 for Cimco-hsm. I do 99% of my mill programming in NX these days. The only time I use MCX is in hard materials for the Cimco adaptive clearing toolpath.

[gcode]

In X2 you'r out out luck...

The 2d High speed in X3 have better control

of this if the bottom surface is flat and the

new dynamic pocket toolpath in X4 looks promising.

As a work around in X2, get the high speed surface toolpath running the way you want it,

then backplot aand save the geometry for the first passes. You can use this to old school

a couple of passes ahead of the main roughing path to remove the material you're worried about.

[neurosis]

quote:

---

(You simply can't get a Surfcam Tru-Mill type path out of Mastercam.) Not true but you need X4 for this.

 

(Maybe X4 will produce acceptable results?) I am thinking so.

 

But the HSM from Cimco is really nice I am playing with this in X4 now.

---

Having used both, in your opinion, which produces better results? X4 or the Cimco-hsm?

 

With the demo of Cimco HSM will it allow you to program and post code to machine a part or is it a crippled demo as most demo's are? I would be interested in giving this a try.

[gcode]

Cimco will give you a fully functioning 30 day trial license. There is a request form on thier website

Cimco HSM

 

They also sell 2 versions now..

The full package contains all thier toolpaths

and a cheaper package that has just the roughing stuff

[cobra95kev]

Neurosis,

When I said I used both I was reffering to Surfcam and the Cimco adaptive clearing (30 day trial). I have not used X4 and might not get to for a while. The place where I am working now doesn't use mastercam, they have V5 only.

[neurosis]

quote:

---

As a work around in X2, get the high speed surface toolpath running the way you want it,

then backplot aand save the geometry for the first passes. You can use this to old school

a couple of passes ahead of the main roughing path to remove the material you're worried about.

---

I am finding even more problems with the path then just the engagement. It spends "allot" of time out of the cut and creates allot of wasted movement. There is also no control to speed the feed up in the areas outside of the cut so I have no control to at least speed the air cuts up to reduce the time spent in those areas. In aluminum this might be ok, but in titanium this makes for allot of air time.

 

quote:

---

Cimco will give you a fully functioning 30 day trial license. There is a request form on thier website

Cimco HSM

---

Thanks! I saw the form. I couldnt find anything that said whether or not it was fully functional or crippled and didnt want to install it unless I could see how it worked in a real situation. I would rather not have to use 3rd party software if at all possible so I am hoping that X4 has addressed some of these shortfalls. Otherwise I think we will have no choice. Its hard to compete with companies that already have this ability.

[neurosis]

quote:

---

Neurosis,

When I said I used both I was reffering to Surfcam and the Cimco adaptive clearing (30 day trial). I have not used X4 and might not get to for a while. The place where I am working now doesn't use mastercam, they have V5 only.

---

That question was aimed at J, Kramer. Sorry for the confusion.

[mchin-pilot]

MC X4 has a toolpath called Dyanmic mill, Is it not like copy of Surfcams true mill. Features like:- Constant engagement angle,microlifts,fast returns.

[Steve Hattori]

Neurosis, Cimco's software runs inside of mcam as a c-hook, and you can create toolbars for it- you get full function and it posts from mcam justlike any mcam toolpath. They will often extend the trial period if you ask. I haven't tried dynamic pocket in

X4 yet, so I don't have direct comparison. I have all of Cimco's toolpath software, and I use it for most 3axis parts, as it produces much smoother high-speed paths, and allows the roughing control you seek. It is such a relief to be able to run a ruf program and never have to touch the speed or feed overrides!...

 

Sorry to dis on mcam in this forum, but a solution to this problem cannot be found in X3..

[neurosis]

quote:

---

MC X4 has a toolpath called Dyanmic mill, Is it not like copy of Surfcams true mill. Features like:- Constant engagement angle,microlifts,fast returns.

---

Sorry, my reading comprehension is bad. I have a hard time interpreting what you are saying here. X4 does have those features or does not?

 

quote:

---

Neurosis, Cimco's software runs inside of mcam as a c-hook, and you can create toolbars for it- you get full function and it posts from mcam justlike any mcam toolpath. They will often extend the trial period if you ask. I haven't tried dynamic pocket in

X4 yet, so I don't have direct comparison. I have all of Cimco's toolpath software, and I use it for most 3axis parts, as it produces much smoother high-speed paths, and allows the roughing control you seek. It is such a relief to be able to run a ruf program and never have to touch the speed or feed overrides!...

 

Sorry to dis on mcam in this forum, but a solution to this problem cannot be found in X3..

---

Does cimco have the ability to change the feed rate while in between cuts to speed up air time? Or does it have the ability to micro-lift as the last guy was saying? I am going to send them an email or call them tomorrow I think. I am going to the x4 roll out today and will be asking allot of these questions about x4. I am very impressed with the true-mill! If cimco even comes close I will be happy. I just hope that it doesnt cost a fortune! Its slow out there right now and getting the boss to spend money is difficult these days.

[gcode]

dynopocketing has micro lift.. the ability to

change feedrates during postioning moves and

multiple retract options and logic switches

to define the retract condtions.

I haven't had the chance to try it on a part yet,

I've used it in a couple of files... they just haven't run them yet.

[cobra95kev]

gcode,

Does it limit the tool engagement angle also?

[neurosis]

And can you limit the lead in and lead out so that it doesnt travel two tool diameters past the edge of the material? (just a little sarcasm)