3d High Speed Machining Toolpaths

[Guest CNC Apps Guy 1]

Books and such are good resources, but lke JP said, you can't ask a book a question.

 

As far as what path to use and when... that's a VERY complicated question to answer. Usually best answered live with someone comfortable with the toolpaths.

[peon]

Daniel, you mentioned you already have experience using the legacy toolpaths. You should be able to just start using the new toolpaths and ask questions as you go along or if you encounter some toolpath movement you are not satisfied with. Some simple advice I can recommend right now is to use boundaries and don't bother too much with check surfaces. You are only gonna learn the toolpaths with practice. Jump in with both feet

[crazy^millman]

I was hoping for some kind of advise from your own personal experience with mastercam. Oh well..

 

Daniel took that totally the wrong way didn't you. There are way to many factor to consider before anyone can suggest the best way for you. I got this tree in my backyard I want cut down. Care to tell me how to do that? Now you go off explaining all I need to do it get a chain saw and cut it at the base. I then go cut down the 400 foot tall tree at the base and destroy my house and 3 others houses. What happened to your advise?

[danielm]

Daniel took that totally the wrong way didn't you. There are way to many factor to consider before anyone can suggest the best way for you. I got this tree in my backyard I want cut down. Care to tell me how to do that? Now you go off explaining all I need to do it get a chain saw and cut it at the base. I then go cut down the 400 foot tall tree at the base and destroy my house and 3 others houses. What happened to your advise?

 

 

Crazy. If you were to name the 5 most common HSM toolpaths that you use, what would they be? What are a few noteable considerations that, in your opinion, is critical for me to understand for each.

 

At this time the feeling that I'm getting is for 2D HST that the Dynamic Area Mill and Peel Mill is pretty popular and would be a logical starting point for me to get familiar with the HSM lingo.

 

For Surface HST, I've heard talk of Area Clearance and Core Roughing mostly for roughing. I don't recall what Surface HST Finishing toolpaths are common favorites. Waterline maybe?

 

 

I'm just trying to make an informed beginning into the world of HSM.....rather than just picking the first one and hoping that I dont end up wishing that I would have started somewhere else. Time is kinda valuable right now.

[peon]

These are the 3 most popular HST I use for molds.

Area Clearance = Surface Rough Pocket

Waterline = Surface Finish Contour (z-level cutting)

Raster = Surface Finish Parallel

[Guest CNC Apps Guy 1]

Daniel, I woudl strongly suggest that if at all possible, take your SIM home with you and spend some time "playing" with the tolpaths. I know that time is a valuable asset, but man, it would be SO worth it. I still do that to this day and I've got darn near 20 years using Mastercam now.

[Redfire427]

Guys. I have been using the old 'stuff' and I need to learn the new 'stuff' as you put it. I'm not hearing about any learning materials that are available. How about something like this: "if you're new to HSM, the best place/toolpath to start learning at is.........." I know that some toolpaths are used more than others as a rule. I need to start there. Problem is I don't know which 'ones' you guys are talking about.

 

Really need some help here...

 

Thanks for any advise!! D

 

Once you get past the anxiety of trying something new, you will actually learn to like the new paths. For simplicity, the toolpaths are broken down into "Roughing toolpaths" and "Finishing toolpaths". That in itself should give you a good starting point. For Roughing, the two that you will likely use the most is Area clearance and core roughing. The two toolpaths have a lot of intelligence and many of the same features, but the easiest way to figure out which one to use come down to whether the part you are trying to cut is shaped more like a cavity ( area clearance ) or more like a boss standing up ( core rouging ). Essentially, area clearance cuts pocketiing passes from the inside toward the outside, and core roughing starts from the outside and works toward the inside. Keep in mind that it is still intelligent enough that if you do have a cavity shape within your model/surfaces, then it will automatically switch strategies and pocket it from the inside toward the outside.

 

 

Opti-rough is a toolpath that utilizes the flutes of and endmill to essentially "peel mill" your 3D model. This is a fairly new approach, yet, it is very effective and is typically used on high-speed machines. If you are using inserted flycutters/feedmill for roughing, this strategy will not work, so stick to the two I mentioned above.

 

Rest rough is basically a toolpath that picks out all the areas that were not addressed with larger tools. Let's say for example you roughed out a cavity shape with lots of detail with a 1-1/2" flycutter. It would be reasonable to assume there is a lot of remaining corners and detail that needs to be picked out prior to finishing. You can choose a much smaller endmill ( say 1/4" ) and it will pick out the areas not cut by the 1-1/2" tool. It will make multiple passes where there is excessive stock.

 

The finishing toolpaths are not that much different than the legacy toolpaths, except they have way more funtionality and control.

 

Carmen

[Jasond0530]

The best way I learnt the new tool paths was to go with what I knew(legacy)! As I am my own programmer/setter and operator(sometimes!)

I would get machine set, go back to the pc and play with the new ones while it was running, once I thought it looked good on screen and time permitting actually run the the new tool paths on part that had already been cut, without coolant! If it looked good run the next one with new paths!

Only problem was having te repost prog with much higher feedrates and shorter cycle times!

[danielm]

Once you get past the anxiety of trying something new, you will actually learn to like the new paths. For simplicity, the toolpaths are broken down into "Roughing toolpaths" and "Finishing toolpaths". That in itself should give you a good starting point. For Roughing, the two that you will likely use the most is Area clearance and core roughing. The two toolpaths have a lot of intelligence and many of the same features, but the easiest way to figure out which one to use come down to whether the part you are trying to cut is shaped more like a cavity ( area clearance ) or more like a boss standing up ( core rouging ). Essentially, area clearance cuts pocketiing passes from the inside toward the outside, and core roughing starts from the outside and works toward the inside. Keep in mind that it is still intelligent enough that if you do have a cavity shape within your model/surfaces, then it will automatically switch strategies and pocket it from the inside toward the outside.

 

 

Opti-rough is a toolpath that utilizes the flutes of and endmill to essentially "peel mill" your 3D model. This is a fairly new approach, yet, it is very effective and is typically used on high-speed machines. If you are using inserted flycutters/feedmill for roughing, this strategy will not work, so stick to the two I mentioned above.

 

Rest rough is basically a toolpath that picks out all the areas that were not addressed with larger tools. Let's say for example you roughed out a cavity shape with lots of detail with a 1-1/2" flycutter. It would be reasonable to assume there is a lot of remaining corners and detail that needs to be picked out prior to finishing. You can choose a much smaller endmill ( say 1/4" ) and it will pick out the areas not cut by the 1-1/2" tool. It will make multiple passes where there is excessive stock.

 

The finishing toolpaths are not that much different than the legacy toolpaths, except they have way more funtionality and control.

 

Carmen

 

 

 

Thats what I'm talkin about!! You just saved me hours of 'click-read-watch-adjust...repeat'. Thanks Carmen!

[Oppiz]

One problem I have with HSM is the programs are big. One on my older machines has limited memory.

[Cuda84]

No spoon for me I just dive right in. If you can use the old ones you can figure out the new ones.

[Allan]

While I find the HSM toolpaths to have great motion, the thing that drives me crazy with the roughing toolpaths is the stock to leave in Z.

The value I set there is never achieved, always more left, sometimes lots more.

I need to check every depth and make sure that it does not leave like .02" when I asked for .004", then play games with the depth cuts regen hope it worked, back to depth cuts adjust again regen hope it worked. Unless you enable the "Add Cuts", but I dont always want that.

I must be the only one who struggles with that, the "old school" toolpaths at least adjusted the depth cut depth so that the stock to leave was consistant.

 

 

Allan

[Matthew Hajicek - Singularity]

Rest Rough doesn't have to come after other paths. I started using it on runners in tapered sprues since the stock is conical (turned), then found you can use it with any stock shape you like. Just set up your stock as a stock model and have at it. I go through a couple sizes of Fraisa high feed endmills alternating between Stock Model and Rest Rough, then give it a finish pass (often Flowline) with a ball. I imagine it would work great for castings and rework / modifications too.

[Ocean Lacky™]

While I find the HSM toolpaths to have great motion, the thing that drives me crazy with the roughing toolpaths is the stock to leave in Z.

The value I set there is never achieved, always more left, sometimes lots more.

I need to check every depth and make sure that it does not leave like .02" when I asked for .004", then play games with the depth cuts regen hope it worked, back to depth cuts adjust again regen hope it worked. Unless you enable the "Add Cuts", but I dont always want that.

I must be the only one who struggles with that, the "old school" toolpaths at least adjusted the depth cut depth so that the stock to leave was consistant.

 

 

Allan

 

A quick and easy work around is a Scallop path set very shallow, say 0 to 10 degrees to knock down any high spots.

 

 

 

[Redfire427]

While I find the HSM toolpaths to have great motion, the thing that drives me crazy with the roughing toolpaths is the stock to leave in Z.

The value I set there is never achieved, always more left, sometimes lots more.

I need to check every depth and make sure that it does not leave like .02" when I asked for .004", then play games with the depth cuts regen hope it worked, back to depth cuts adjust again regen hope it worked. Unless you enable the "Add Cuts", but I dont always want that.

I must be the only one who struggles with that, the "old school" toolpaths at least adjusted the depth cut depth so that the stock to leave was consistant.

 

 

Allan

 

Allan, I hear your complaint. What I do to address this issue is immediately after using area clearance or core roughing, is to follow it up with a horizontal finishing toolpath to get the same stock on the floors as I have on the walls. Unlike the legacy tolpaths that have "detect flats", you are on your own to come up with something that works. "add cuts" is only used to get more detail on fillets or shallow angled areas. I wouldn't use it unless absolutely necessary due to the ridiculous calculation times and also it will usually add that cut around the entire model which will kill your machining time.

 

Carmen

[Jeremy Herron@DBS Solutions™]

While I find the HSM toolpaths to have great motion, the thing that drives me crazy with the roughing toolpaths is the stock to leave in Z.

The value I set there is never achieved, always more left, sometimes lots more.

I need to check every depth and make sure that it does not leave like .02" when I asked for .004", then play games with the depth cuts regen hope it worked, back to depth cuts adjust again regen hope it worked. Unless you enable the "Add Cuts", but I dont always want that.

I must be the only one who struggles with that, the "old school" toolpaths at least adjusted the depth cut depth so that the stock to leave was consistant.

 

 

Allan

 

 

I trick mentioned the other day in another thread, use the opticore/ area/ or rest and set your step up value to match your step down and it will cut the flat areas leaving the amount of stock in z you set.

[Jason @ CPM Industries]

Does anyone know the best filter settings for a haas?

Refine toolpath is on.

Arc's in all planes.

Toolpath tolerance is .0005

Not sure why but the slide bars

in the refine page don't stay were you put them.

[gms1]

While I find the HSM toolpaths to have great motion, the thing that drives me crazy with the roughing toolpaths is the stock to leave in Z.

The value I set there is never achieved, always more left, sometimes lots more.

I need to check every depth and make sure that it does not leave like .02" when I asked for .004", then play games with the depth cuts regen hope it worked, back to depth cuts adjust again regen hope it worked. Unless you enable the "Add Cuts", but I dont always want that.

I must be the only one who struggles with that, the "old school" toolpaths at least adjusted the depth cut depth so that the stock to leave was consistant.

 

 

Allan

 

I'm with you here Allan. I really hate typing a number in a box then getting something completely different. Yeah there's tons of things you can do after you get that arbitrary depth but I'd rather the toolpath follow my actual numbers.