What's new
What's new

For people who have experience in camworks multiaxis - 5 axis

motox2121

Plastic
Joined
Nov 16, 2020
Hi All -

We made the jump this year to 5 axis milling - I have a lot of experience designing inside of solidworks, and am very used to the interface, so I wanted something that integrated into solidworks. I have used mastercam for solidworks in the past - years ago, and had some success. It seems like a lot of the local guys use Camworks / Solidworks CAM, but most are not doing any 5 axis milling. We purchased Camworks with the full blown simultaneous package - We got up and running pretty quickly, but there is definitely some quirky behavior in the software. For the most part, I can get things done, but sometimes the multiaxis stuff requires a lot of workarounds / surface offsets / trimming to get what I want. I feel like I am constantly tricking the software into getting the results I need. I notice buggy behavior quite a bit. Tech support has been good, but a lot of the time they cant even explain the "why" behind the bugs I am seeing.

For those of you who program 5 axis mills - I am curious if you have used Camworks before with success? If so - have you since switched to a more "advanced" software? i.e. Hypermill? Also Mastercam with the 5 axis deburring module looks awesome... Even basic fusion has some things that look appealing to me.

Just curious how this platform compares to others, it seems more geared towards 2.5 / 3 axis stuff, but I don't have too much to compare too. I love the fact it uses SW tools / interface.

Looking for feedback specifically in the multiaxis realm. I feel like I am constantly dicking around with settings, guessing and checking to get the results I want. Some settings dont scale how you would expect them to, and even after a year inside the software, it still does not feel intuitive. We are making some complex parts with simultaneous toolpaths, but the time it takes to get the result we are seeking, is too high for now.

I know this will come with time and experience, but I am looking for some feedback from someone who has ran Camworks 5 axis as well as other higher end software packages, and can give me feedback between them. Camworks is definitely powerful, but some things could be improved for sure. I don't want to invest crazy time into it if it is not the right option. It seems everyone complains about their software in some way.

Thank you !
 

Chris59

Cast Iron
Joined
Nov 28, 2006
Location
Jupiter, Florida
I feel like I am constantly dicking around with settings, guessing and checking to get the results I want. Some settings dont scale how you would expect them to, and even after a year inside the software, it still does not feel intuitive.

We don't do 5 axis but we do 4 axis with undercuts that uses the 5 axis module. I agree, the 5 axis interface is a lot of trial and error even at my low level.
I like Camworks (I have used OLDER versions of Mastercam and Smartcam) but the 5 axis module is my weak spot. Following this.
I hope you get real information instead of fan boys for their own CAM systems.
 

BluishInventor

Aluminum
Joined
Jul 7, 2020
I've been using Camworks for the last 3 years... and I haven't been too impressed. The potential for it to be great is quite huge, but the lack of focus on squashing bugs and streamlining workflows leaves me wanting more. I as well have been using SW for some time and having CW integrated is a blessing and a curse. The associativity of features to the geometry is nice because if you are working with the same files the designers are using, if they make a change it's a simple regenerate command(mostly simple) and your toolpath gets updated. But the SW back end can only handle so much. Solidworks Has Encountered a Problem comes to mind.

Personally, I've struggled to be effective with any of the 3 axis toolpaths when it comes to stitching surfaces as well as the 5 axis module. This and some other features that it is lacking is driving me elsewhere. So, I've been evaluating different CAM systems for the last month or so to see if something will suit our needs a bit better in that department.

Mastercam and Edgecam use the same 5 axis module that Camworks does, which is created by Moduleworks. However, while Edgecam implements it almost exactly like Camworks, Mastercam breaks it up into specific toolpaths which makes it simpler to get a toolpath that is desirable from the get-go. Then yesterday I was presented with a Hypermill demo(which they do all their own pathing algos) and it literally towers over anything I've seen when it comes to 5 axis. And by this I mean you can get super clean paths and really trick toolpaths with little user interaction. To me, that's huge. With Camworks I also have to do a TON of trial and error to get anything remotely close to usable. Hell, on a external fillet that I wanted to hemstitch(one that you could do with a corner rounder) I struggled to get a smooth toolpath and ended up reaching out to support(Hawkridge). They reproduced it on a generic part they made and found a solution, but that solution didn't work on my part. And that's where that ended.

But back to the 5 axis operation in Camworks. I've learned that instead of using the Swarf Mill pattern, just use the regular milling pattern with 5 axis and the Cut Relative to Surface set to 90 degrees is a better option. Combine that with the driving curve set to Offset from Curve and then set your Number of Cuts to 1. You get a few more options doing it this way than you would with the Swarf pattern. It's a silly workaround, but again that's what Camworks is good at... work arounds. :rolleyes5:

Screenshot 2021-05-20 071753.jpgScreenshot 2021-05-20 071831.jpg

But to really be efficient with the Camworks module, you just got to get through that learning curve. Learning the Axis Control tab is essential and then implementing Gouge checking with just the flue/shank and using the Tilt Tool strategy there to minimize retracts. Linking is also a pain because it's hit or miss when it gives you results that are desirabled. I haven't really dove into the Roughing tab, but when I have it's another hit or miss type deal where sometimes the path looks good and other times you're like "wtf are you doing CW?". I wish I could help more here but I feel the 5 axis module is too finicky and specific and I would need to see an example you are struggling with before I could give any useful advice.

But you are not alone here. I would utilize your reseller if you can. Hawkridge has a couple pretty savvy 5 axis CW users that can trouble shoot the majority of issues quickly. For me, if I have to spend more than 15 minutes muckin' around with a toolpath, then I'm losing money. I pass it off to them and say "Why isn't this giving me results." Usually its one or two unsuspecting parameters that need to be just right. Sometimes it's a work-around. But rarely is it because I don't know how to use the dialogue because any time we do a gotomeeting and they drive the mouse, they just repeat everything I've done and said they will need to mess around with the file on their end. An hour or two later, I get an answer. So, it's 2 hrs they spent on the issue and I just continue on with my day and implement their solution once they get back to me. It's not intuitive by any means, which is not good for those that have 5 axis experience and they know what they want to do. It's just a flat out pain to get nice, clean toolpaths. IMO

If you can share a specific example, I may be able to help further. Until then, I can really only say good luck.
 

Shawnrs

Stainless
Joined
Mar 30, 2016
I have used it before but that was a 6 or 7 years ago when we had a 5 axis machine. I can say get training on it because it is different from the standard packages. I used mostly the multi surface feather (5 axis) option for almost all the machining. I think the hardest part is getting your coordinate systems set up.
 

motox2121

Plastic
Joined
Nov 16, 2020
Yes - hoping there are some users on the board. The deeper I get into it, it seems like there is not a huge camworks user base, even with SW buying it out for their CAM (or maybe just licensing it).

If the support is not there for the high end stuff long term, I will be moving away from this and going to another software package that is focused on quick workflows and clean solutions.
 

motox2121

Plastic
Joined
Nov 16, 2020
I have used it before but that was a 6 or 7 years ago when we had a 5 axis machine. I can say get training on it because it is different from the standard packages. I used mostly the multi surface feather (5 axis) option for almost all the machining. I think the hardest part is getting your coordinate systems set up.

I am good with the WCS - and am using the multisurface features with 5 axis mill toolpaths. The challenge is the interface, not much explanation as to what each setting does, even in the help file. They say a basic overview, but do not explain the interrelationships between all of the different variables. It is very much trial and error.

Thanks -

Are there any high level camworks users on this board ?
 

Shawnrs

Stainless
Joined
Mar 30, 2016
I am good with the WCS - and am using the multisurface features with 5 axis mill toolpaths. The challenge is the interface, not much explanation as to what each setting does, even in the help file. They say a basic overview, but do not explain the interrelationships between all of the different variables. It is very much trial and error.

Thanks -

Are there any high level camworks users on this board ?

At the time I was trained on the 5 axis software Camworks was pretty green with it. Today I think it is better but I rarely use that since we do not have a 5 axis anymore. The 5 axis option I use is good for surfacing parts I something program. As for high level camworks users on this board I would say there a few of us but not many that post on here.
 

motox2121

Plastic
Joined
Nov 16, 2020
I am having some issues getting some smooth code coming out of simultaneous multiaxis mill - flowline between curves pattern, and tilted relative to cutting direction 5-axis control. Toolpath looks great but I get some jerky motion, A axis bouncing back and forth instead of a smooth transition. If anyone is well experienced with this stuff please let me know. I usually have to do a tilt through curve axis control option and create a bunch of construction geometry, and sometimes have to create new surfaces to get what I need, which takes a lot of time. If I can get the tilted relative to cutting direction smoothed out, that would help my workflow out immensely.

Let me know if anybody has good experience, have a toolpath that has been driving me nuts trying to get it perfect.
 

BluishInventor

Aluminum
Joined
Jul 7, 2020
The one thing I actually like about CW is the simulation. Not virtual machine, but the built-in simulation. When you simulate the toolpath, you can turn on the tool axis and the should appear as yellow lines sticking up from the toolpath representing the tool's axis. You can set these lines to show up leading and trailing the current tool position. Depending on the number of angle changes, you can set it to either 10, 30, or 50. I usually use 10-30 of these lines leading and trailing the current position. These lines will make the odd/jerky type moves more apparent. It doesn't solve the problem, but helps identify it.

What I found to be really helpful in the jerky movements is a parameter, I can't remember the exact one as I'm not at my computer but I copied the description of it from another user's post that explains it well. The option 'lets you select between Ortho to cut direction at each position which is default. Changing to Follow surface ISO direction provides pretty smooth motion in my experience, depending on surface tolerance setting.' They were talking about mastercam which uses the same module works algos as camworks and the parameter options and pictures are nearly identical. The only thing mastercam does is split up the 5 axis toolpath strategies into separate operation types whereas camworks keeps it all in one. Edgecam is the same way.

Also, look into the Minimum angle change too. It helps, but not as much as Following the Surface ISO direction.
 

thesidetalker

Hot Rolled
Joined
Jan 11, 2015
Location
Bay Area, CA
The one thing I actually like about CW is the simulation. Not virtual machine, but the built-in simulation. When you simulate the toolpath, you can turn on the tool axis and the should appear as yellow lines sticking up from the toolpath representing the tool's axis. You can set these lines to show up leading and trailing the current tool position. Depending on the number of angle changes, you can set it to either 10, 30, or 50. I usually use 10-30 of these lines leading and trailing the current position. These lines will make the odd/jerky type moves more apparent. It doesn't solve the problem, but helps identify it.

What I found to be really helpful in the jerky movements is a parameter, I can't remember the exact one as I'm not at my computer but I copied the description of it from another user's post that explains it well. The option 'lets you select between Ortho to cut direction at each position which is default. Changing to Follow surface ISO direction provides pretty smooth motion in my experience, depending on surface tolerance setting.' They were talking about mastercam which uses the same module works algos as camworks and the parameter options and pictures are nearly identical. The only thing mastercam does is split up the 5 axis toolpath strategies into separate operation types whereas camworks keeps it all in one. Edgecam is the same way.

Also, look into the Minimum angle change too. It helps, but not as much as Following the Surface ISO direction.

Yea that is another good one. Minimum angle change.

On Surfcam its called "Maximum Angular Departure" which it basically divides the angular moves into smaller, equal segments until they are under this value. (default of 3° and Ortho doesn't make equal angular moves I've found)

I find around 0.4 works good for me, in most cases.

I discovered that when trying to mill a vacuum groove across some flat and curved surfaces with the tip of a square endmill. Not only does the smaller value produce smaller angular movements (and smoother motion) but with larger angular values the tool will tilt across the flat sections leading up to and away from the angular moves. Once the value is small enough, it seems to respect the flats and prevent gouging (or leaving excess material with gouge checking on).

Assuming CamWorks has similar option hidden in there somewhere...? Module Works right?

Smaller angular moves should still help smooth the motion a bit even using through-curve for vector control, I'd think.
 

motox2121

Plastic
Joined
Nov 16, 2020
Yep - I have played with I think every parameter - I have minimum angle change set to 0.1 , and have played with ortho / follow surface ISO. What worked best for me on this application was change to fixed angle relative to Z, which was OK for this application but not every application I think. I was able to get really nice motion and ended up with a beautiful part. The software is powerful but I feel the interface does not give you the tools to figure out the relationships between settings. You just have to know from trial and error experience, the help file is not amazing and there is not much online for video tutorials other than goengineer, which I am thankful for.
 

thesidetalker

Hot Rolled
Joined
Jan 11, 2015
Location
Bay Area, CA
In your previous post, you mention A-axis bouncing back and forth. How much was it?

Are you getting small tilt-axis moves back and forth when it should be constant?
 

motox2121

Plastic
Joined
Nov 16, 2020
In your previous post, you mention A-axis bouncing back and forth. How much was it?

Are you getting small tilt-axis moves back and forth when it should be constant?

Yes Exactly, It looks like just a bunch of unnecessary tool reorientation moves that oscillates in certain areas It is a simple path but the tilt strategy is going a bit nuts it looks like. I'm not sure how much of this is handled on the posting side or if it is all driven from the CAM side. d

Also noticed sometimes several lines of A motion or C motion in a row, with no other x y or z moves. Simply:

A92.
A93
A90

Etc then resumes with normal simultaneous. I believe this could be post related too, but looking for a way to smooth this out. Could totally be a setting thing but my VAR could not figure out what was causing it.

If you have any ideas - please let me know. As I said, it looks like it is a code issue and not a machine issue.
 

thesidetalker

Hot Rolled
Joined
Jan 11, 2015
Location
Bay Area, CA
I ask because I too get small oscillations on tilt-axis at times, when it should be constant. Again, different software, but still moduleworks, right?

I would get ±.005° or so, randomly. I "filter" this out with my post, using a .01° threshold. I have my posts simply leave out these small angular moves unless the movement is .01 or larger from the last used address. Technically not correct, but in the grand scheme of things I don't think it affects the work I do all that much. If I remember right, I think it did help reduce some jerky motion, however it has been a long time since I experimented with this though.


The biggest difference I noticed in reducing jerky motion is if the angular moves are of similar size. That's where the angular tolerance helped.

Doing a simple swarf test right now, using default tolerance of 3° - the C-angles will be consistent for a few lines of code at a time, but vary a lot. from 1.5 up to 2.6°

Using tolerance of 0.4° - every single line of code is exactly 0.352

NC file is much larger and more lines of code, but the control runs it smoother as it is a constant speed.



Also noticed sometimes several lines of A motion or C motion in a row, with no other x y or z moves. Simply:

A92.
A93
A90


How does the rest of your program look? Line to line, what are the changes in both A/C? If it varies a lot line to line it probably wont be smooth motion. And do you see those tilt-only moves in CAM in backplot/sim?
 

motox2121

Plastic
Joined
Nov 16, 2020
I ask because I too get small oscillations on tilt-axis at times, when it should be constant. Again, different software, but still moduleworks, right?

I would get ±.005° or so, randomly. I "filter" this out with my post, using a .01° threshold. I have my posts simply leave out these small angular moves unless the movement is .01 or larger from the last used address. Technically not correct, but in the grand scheme of things I don't think it affects the work I do all that much. If I remember right, I think it did help reduce some jerky motion, however it has been a long time since I experimented with this though.


The biggest difference I noticed in reducing jerky motion is if the angular moves are of similar size. That's where the angular tolerance helped.

Doing a simple swarf test right now, using default tolerance of 3° - the C-angles will be consistent for a few lines of code at a time, but vary a lot. from 1.5 up to 2.6°

Using tolerance of 0.4° - every single line of code is exactly 0.352

NC file is much larger and more lines of code, but the control runs it smoother as it is a constant speed.






How does the rest of your program look? Line to line, what are the changes in both A/C? If it varies a lot line to line it probably wont be smooth motion. And do you see those tilt-only moves in CAM in backplot/sim?

When you say "Filter" do you mean apply angle tolerance? Or do you have a custom post function that filters this ? Swarf paths are where I can see wild differences in motion using different angle tolerance settings.
 

thesidetalker

Hot Rolled
Joined
Jan 11, 2015
Location
Bay Area, CA
When you say "Filter" do you mean apply angle tolerance? Or do you have a custom post function that filters this ? Swarf paths are where I can see wild differences in motion using different angle tolerance settings.

Yes custom post function. It simply keeps the tilt axis the same if the difference from previous to current value is <.01
 

BluishInventor

Aluminum
Joined
Jul 7, 2020
I just want to jump in here and say that I was advised by our reseller and their best 5-axis guy to NOT use the swarf mill option as the Pattern type.

Instead, use Milling as the type, then use Offset from Curve(select the bottom curve of the wall you are trying to swarf). Also, at the bottom of the pattern tab, set to By No of Cuts and set it to 1.

Then on the Axis control tab, use 5 axis, and set 'The Tool Axis Will Be' option to Tilted Relative to Cutting Direction and set the tilt to 90 deg. This is effectively the same path as swarf, but you get so much more control and options in tweaking it to be nice.

You may want to start a fresh operation if you have messed with the parameters a bunch so that you know where you start.
 

motox2121

Plastic
Joined
Nov 16, 2020
I just want to jump in here and say that I was advised by our reseller and their best 5-axis guy to NOT use the swarf mill option as the Pattern type.

Instead, use Milling as the type, then use Offset from Curve(select the bottom curve of the wall you are trying to swarf). Also, at the bottom of the pattern tab, set to By No of Cuts and set it to 1.

Then on the Axis control tab, use 5 axis, and set 'The Tool Axis Will Be' option to Tilted Relative to Cutting Direction and set the tilt to 90 deg. This is effectively the same path as swarf, but you get so much more control and options in tweaking it to be nice.

You may want to start a fresh operation if you have messed with the parameters a bunch so that you know where you start.

Thanks man ! This in theory sounds really great. Makes total sense. I also found on the path I was having issues with (surfaces were interrupted with some slots) - I created a new surface that was uninterrupted, and the resulting path was clean with the swarf path. I would not have known that without randomly trying it, trying to figure things out.

Appreciate that tip ! Who is your reseller?
 

BluishInventor

Aluminum
Joined
Jul 7, 2020
Hawkridge. They do a pretty stellar job across the board both for Solidworks and Camworks.

So, for the 'continuous feature' or surface, I understand your pain. But do try to avoid that if possible as it's extra work. And once you get a good path be sure to either save a new default parameter setting or save an operation plan. I prefer the default parameter setting, but remember it's only for that specific feature type. Since it's a multi-surface feature, that's pretty easy to re-use going forward. For all the other feature types... good luck. lol.
 

5 axis Fidia guy

Stainless
Joined
Aug 17, 2006
Location
Wisconsin
It seems as though everyone has a gripe in their software of some sort. I have been a Powermill user for the past 25 years and can honestly say there is nothing I cannot do with it on our 5x machines. Hypermill has always been interesting to me but I never got to serious about it. I just read the "what's new" section in Hypermill 2021.1 and everything it added Powermill can do, and some of it for years. I know a Hypermill guru quite well and he summed it up like this. Hypermill can sometimes give you the cleanest toolpath right out of the gate, but Powermill is hands down the king when it comes to toolpath editing and modifying AFTER calculation. Honestly the biggest downer in Powermill is Autodesk got their hands on it.
 








 
Top