Community
Fusion Manufacture
Talk shop with the Fusion (formerly Fusion 360) Manufacture Community. Share tool strategies, tips, get advice and solve problems together with the best minds in the industry.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

A short list of Fusion Turning features that either don't exist or don't work properly

3 REPLIES 3
Reply
Message 1 of 4
steveHDPJT
166 Views, 3 Replies

A short list of Fusion Turning features that either don't exist or don't work properly

First, what happened to the idea station for Fusion? Did that get taken down or moved somewhere? I did actually look before posting but couldn't find anything.

 

Anyway, here are a number of things that frequently trouble us with Fusion, primarily with turning albeit some mill-related stuff (using a Nakamura lathe with live tooling and Y axis):

 

  1. Lathe tool and holder definitions, in the rare instances that they exist, suck across the board.
  2. Live tool holders don't exist at all and there are no real workaround options for them. Need to be able to have the post determine whether the tool holder should go forwards or backwards
  3. Lack of associativity between cloud and document level tool libraries makes it seemingly impossible to actually keep on top of lathe tools. 
  4. Can't specify to force C axis or Y axis output at the Operation level. Can do it in the post, but it affects all operations that way, and it should just be a tick box in the Operations menu.
  5. Form/step drills don't exist as a tool type. Can use a form mill for drilling but doesn't simulate properly.
  6. If you use a drilling op with an end mill, for some reason "feed per revolution" tickbox disappears and it outputs in feed/min.
  7. No form tools or solid carbide turning tool profiles exist.
  8. Can't specify feed rate by line segment. This is quite annoying for things like grooving or anything where you're using a sharp corner (or very small TNR) for a chamfer. Fanuc MGi lets you do this kind of thing at the control segment by segment - it's both faster AND far more powerful than Fusion for turning.
  9. Threads (modeling, drawings and CAM) are universally terrible. Besides not allowing custom thread sizes, the Major/Minor diameters don't reflect reality and can't be controlled. Nothing gets automatically calculated except the major of male threads and minor of female threads. No mention of pitch diameters exists. Specification of turned or thread-milled dimensions is done very indirectly (as a radial offset from the Fusion-generated major/minor diameter) with no option to simply tell it "this is the final diameter the tool must reach" or "this is the pitch diameter I want". We do a lot of aluminum work where parts get anodized after machining, which requires specific allowances for thread dimensions. All of this has to be done manually to get around the roadblocks that Fusion creates.
  10. Threading (or in our case thread chasing) with a single point turning tool doesn't work properly if you specify only one pass. It decides that the cycle time for that operation will be some 10 figure number of seconds.
  11. Threading clearance radius doesn't work if you just give it a diameter input (at least, if the diameter is smaller than the stock diameter). It does work if you select a surface and then choose to offset from that.
  12. Would be nice if there was some option to link thread chasing to the initial threading pass for single point threading, so that if anything is adjusted, both are updated. Kind of like a pattern system, but where the thread chase op is automatically generated using the same values but with only one pass, and it asks you to put a thread clip turning op in between the two. For single point threading it's pretty common to turn/thread/clip/chase and it'd be sweet to have some automated cycle for that.
  13. Machine definitions for turning may as well not exist. You select a whole lot of input data and absolutely nothing comes of it. It should let you determine which direction positive Z is for each spindle, as well as which direction the C axis rotates for that machine. Doing it in the post is a friggin nightmare.
  14. For some reason when posting stuff out using a post that's in a linked Google Drive folder, certain values revert to random things that are utterly inexplicable to me. For example, we have a custom property called PickoffLength for automating the stock transfer between spindles. The default value that's saved in the post is 5mm. If I set it to 7mm and post a program, the next time I come back to repost the same program it's changed the value to 20mm for no reason I can determine (it shows up blue as though it's been modified from the default value, but it hasn't by me!). This is obviously extremely dangerous. I want the computer to automatically check my work, not require manual checking of the computer's work when it's repeating the same thing it was just asked to do!
  15. Most Fanuc based machines have servo torque detection options, for example to check whether a tool still exists or not. Would be nice to have some way to command it to do that through CAM (kind of like probing) without having to manually input it each time.

All of the above are things I think can be addressed without setting the world off its axis, but I have a couple of BIG suggestions that might be huge projects:

  1. Lathe simulation incl turret would be nice. Be really good if you could 3D-scan the inside of your machine and have it automatically determine your tool stickouts etc to detect collisions.
  2. How hard would it be to have a reverse post processor that takes in your modified-at-the-control program, imports it back into Fusion and actually corrects the CAM programming to match it? Because there are many, many things that Fusion simply cannot do with turning, that we do by hand instead, and there is a lot of fine-tuning that happens at the control because changing a feed rate there takes 2 seconds intead of 10 mins to adjust the program, repost, re-send to machine etc, but we want to bring it back into CAM so that the template can be used for other similar parts. Or at least some kind of version control would be nice.
3 REPLIES 3
Message 2 of 4
Garrett_Wade
in reply to: steveHDPJT

While #4 would be cool to just be there by default....if I understand what you are asking for correctly, it's currently possible for you to have your exact request today with a minor post edit and using operation properties instead of post properties for that setting.
Message 3 of 4
seth.madore
in reply to: Garrett_Wade

And #4 can also be triggered by using a ManualNC "Action" item for "usePolarMode" (or some such text, it varies per post processor)


Seth Madore
Customer Advocacy Manager - Manufacturing
Message 4 of 4
seth.madore
in reply to: steveHDPJT

@steveHDPJT thank you for posting here and sharing your pain points as they relate to tools and Turning in general, it is appreciated! I'll try to address these points by topic (some are tool library, others are turning specific).

Right off; we retired the IdeaStation many years ago as our backlog of work was ever growing and we also have a very open community and an engaged MFG forum. We've got no shortage of new ideas coming in on a daily basis, (drinking from a firehose, one might say..)

 

(please understand if some of my responses are vague, there are somethings I'm legally bound to keep "under wraps")

 

Let's start off with your thoughts as they relate to tooling/tool library:

 


@steveHDPJT wrote:
  1. Lathe tool and holder definitions, in the rare instances that they exist, suck across the board.
  2. Live tool holders don't exist at all and there are no real workaround options for them. Need to be able to have the post determine whether the tool holder should go forwards or backwards
  3. Lack of associativity between cloud and document level tool libraries makes it seemingly impossible to actually keep on top of lathe tools. 
  4. ...
  5. Form/step drills don't exist as a tool type. Can use a form mill for drilling but doesn't simulate properly.
  6. If you use a drilling op with an end mill, for some reason "feed per revolution" tickbox disappears and it outputs in feed/min.
  7. No form tools or solid carbide turning tool profiles exist.

1) Yep, lathe tools (as default) are rather poor. We tossed some examples in their and expected left our customers to their own devices. We have work in-progress to improve upon this.

 

2) No, live tool holders and how we represent them is almost non existent. There is ongoing work to accurately reflect such holders, but that work is much more "long term" and likely not to result in something "customer facing" for quite some time. We're not ignorant of the customer needs (I myself have a shop and a Doosan Lynx 2100), it's just a matter of laying all the foundational work

 

3) No, there is no associativity between document and main library. This is something we would like to address at some point in the future, but nothing is planned in this area for the foreseeable future (to my knowledge)

 

5) Can you expand on this? If I make a step drill and drill a hole, it does reflect the shape of the form tool:

2024-03-08_05h28_34.png

 

6) I'll have to investigate this, that sounds like a small bug.

7) This is something we're also keenly aware of and it IS on our shorter term roadmap (although still quite a ways off, likely not to be seen anytime soon though)

 

Alright, let's take a look at your thoughts on toolpaths and related:

 


@steveHDPJT wrote:
  1. ...
  2. ...
  3. ...
  4. Can't specify to force C axis or Y axis output at the Operation level. Can do it in the post, but it affects all operations that way, and it should just be a tick box in the Operations menu.
  5. ...
  6. ...
  7. ...
  8. Can't specify feed rate by line segment. This is quite annoying for things like grooving or anything where you're using a sharp corner (or very small TNR) for a chamfer. Fanuc MGi lets you do this kind of thing at the control segment by segment - it's both faster AND far more powerful than Fusion for turning.
  9. Threads (modeling, drawings and CAM) are universally terrible. Besides not allowing custom thread sizes, the Major/Minor diameters don't reflect reality and can't be controlled. Nothing gets automatically calculated except the major of male threads and minor of female threads. No mention of pitch diameters exists. Specification of turned or thread-milled dimensions is done very indirectly (as a radial offset from the Fusion-generated major/minor diameter) with no option to simply tell it "this is the final diameter the tool must reach" or "this is the pitch diameter I want". We do a lot of aluminum work where parts get anodized after machining, which requires specific allowances for thread dimensions. All of this has to be done manually to get around the roadblocks that Fusion creates.
  10. Threading (or in our case thread chasing) with a single point turning tool doesn't work properly if you specify only one pass. It decides that the cycle time for that operation will be some 10 figure number of seconds.
  11. Threading clearance radius doesn't work if you just give it a diameter input (at least, if the diameter is smaller than the stock diameter). It does work if you select a surface and then choose to offset from that.
  12. Would be nice if there was some option to link thread chasing to the initial threading pass for single point threading, so that if anything is adjusted, both are updated. Kind of like a pattern system, but where the thread chase op is automatically generated using the same values but with only one pass, and it asks you to put a thread clip turning op in between the two. For single point threading it's pretty common to turn/thread/clip/chase and it'd be sweet to have some automated cycle for that.
  13. ...
  14. ...
  15. ...

asdasd

 

4) As I (and others) mentioned earlier, this is already possible with either minor post hacks or a Manual NC "Action".

 

8.) I agree, feedrate control has long been lacking in turning, for the same reasons you raise. I'll chat with the development team to see if there are any near-term goals for this. Based on what I know, I'm inclined to suspect there are no active projects to address this.

 

9) There is active work (at least on the MFG side) to make Threads more palatable. Yes, I agree, we're very limited right now. This is a bigger project than one might expect, so it's not going to be a quick solution. That said, I've seen the direction we're heading regarding threads and I suspect you will be quite satisfied with the MFG solutions we're working on.

 

10) This was fixed in the update that went out yesterday

11) Hmm, I don't think I've noticed that, let me investigate and see, that sounds like a bug

12) This does sound like a nice QoL item, as it certainly is a common workflow. All I do when I program threads is to duplicate the toolpath and remove the multiple passes.

 

Moving on to machine sim and posting issues:

 


@steveHDPJT wrote:

 

  1. ...
  2. .
  3. .
  4. .
  5. .
  6. .
  7. .
  8. .
  9. .
  10. .
  11. .
  12. .
  13. Machine definitions for turning may as well not exist. You select a whole lot of input data and absolutely nothing comes of it. It should let you determine which direction positive Z is for each spindle, as well as which direction the C axis rotates for that machine. Doing it in the post is a friggin nightmare.
  14. For some reason when posting stuff out using a post that's in a linked Google Drive folder, certain values revert to random things that are utterly inexplicable to me. For example, we have a custom property called PickoffLength for automating the stock transfer between spindles. The default value that's saved in the post is 5mm. If I set it to 7mm and post a program, the next time I come back to repost the same program it's changed the value to 20mm for no reason I can determine (it shows up blue as though it's been modified from the default value, but it hasn't by me!). This is obviously extremely dangerous. I want the computer to automatically check my work, not require manual checking of the computer's work when it's repeating the same thing it was just asked to do!
  15. Most Fanuc based machines have servo torque detection options, for example to check whether a tool still exists or not. Would be nice to have some way to command it to do that through CAM (kind of like probing) without having to manually input it each time.

All of the above are things I think can be addressed without setting the world off its axis, but I have a couple of BIG suggestions that might be huge projects:

  1. Lathe simulation incl turret would be nice. Be really good if you could 3D-scan the inside of your machine and have it automatically determine your tool stickouts etc to detect collisions.
  2. How hard would it be to have a reverse post processor that takes in your modified-at-the-control program, imports it back into Fusion and actually corrects the CAM programming to match it? Because there are many, many things that Fusion simply cannot do with turning, that we do by hand instead, and there is a lot of fine-tuning that happens at the control because changing a feed rate there takes 2 seconds intead of 10 mins to adjust the program, repost, re-send to machine etc, but we want to bring it back into CAM so that the template can be used for other similar parts. Or at least some kind of version control would be nice.

13 and A.) Machine Definitions and total machine simulation is an area we are heavily focused on. Again, it's something that's still a ways off, but we are actively working on solving this.

 

14) This sounds like a bug. Can you make a separate thread that goes into detail and share examples/recording of this happening?

 

15) This would likely be easy to implement with an Operation Property in your post processor. An Operation Property would show up in your actual toolpath dialog as a new tab. It's quite powerful when implemented correctly.

 

Lastly; B) Extremely difficult. There are changes that one could do in the g-code that simply don't convert into something the software would understand.


Seth Madore
Customer Advocacy Manager - Manufacturing

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums