We added support for setting mills/drills as live/non-live tools in HSMWorks 2017. Before the mill-turn posts would automatically guess if live versus non-live mode was desired. However, with the new setting the user is fully in control is the intended behavior without having to make changes to the posts. The live setting only applies to lathes. Ie. the tool is mounted static (no spindle) in your turret.
When creating new mills/drills the default is "live". So if you want to drill with a static/non-live tool you would need to explicitly turn off the live setting in the tool library. The setup sheet will also specify if a tool is live/non-live.
You would use a non-live tool when drilling on the lathe rotary axis. Drilling of axis would require a live tool.
Snippet from Setup Sheet:
Inventor HSM should have it soon. Fusion will take a bit longer.
The live-tool support will be available in the next update of Inventor HSM which will be coming very soon (next couple weeks).
As @fonsecr mentioned, it will be a little longer for Fusion, but still should be supported soon.
Hope this helps.
Noah
@balsmen wrote:
The live-tool support will be available in the next update of Inventor HSM which will be coming very soon (next couple weeks).
As @fonsecr mentioned, it will be a little longer for Fusion, but still should be supported soon.
Hope this helps.
Noah
Thanks for the info @balsmen !
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
Its kind of confusing to see this option when you are defining a tool for a mill, since there is no concept of a live tool on a mill.
From what is posted in here, there would be no end-result to changing this setting for a 3-axis milling tool.?
@rathomas.mobile wrote:
Its kind of confusing to see this option when you are defining a tool for a mill, since there is no concept of a live tool on a mill.
From what is posted in here, there would be no end-result to changing this setting for a 3-axis milling tool.?
Indeed, wouldn't change anything when just programming for a mill.
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
Hi @fonsecr. I really like this option, but I've seen multiple occasions where the customer by accident did program an axial centerdrilling toolpath as livetool. Most of the time they see it on time om the machine, but its a risk.
Could there be a warning/notification while postprocessing (think its hard to make this happen inside inventor/fusion) if you have axialcenterdrilling+livetool for every millturn post?
Inventor HSM and Fusion 360 CAM trainer and postprocessor builder in the Netherlands and Belgium.
@ArjanDijk wrote:
Hi @fonsecr. I really like this option, but I've seen multiple occasions where the customer by accident did program an axial centerdrilling toolpath as livetool. Most of the time they see it on time om the machine, but its a risk.
Could there be a warning/notification while postprocessing (think its hard to make this happen inside inventor/fusion) if you have axialcenterdrilling+livetool for every millturn post?
Actually, I would expect all the axialCenterDrilling logic to be totally removed from all the stock posts.
Since it wouldn't be needed anymore.
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
Hi @Laurens-3DTechDraw. Even if thats the case you'll see that a non driven tool is selected, you hear the internal motor run and the tool will jam into the part. So something like
if(machineState.liveToolIsActive && machineState.axialCenterDrilling){
promptKey2("Livetool", "Watch out: Livetool selected with AxialCenterdrilling", "OC");}
Inventor HSM and Fusion 360 CAM trainer and postprocessor builder in the Netherlands and Belgium.
Sorry, but to me this feels like can't the system tell me in the machine there is a tool diameter 40 but I selected a diameter 5 in the CAM.
I mean you select a live tool, so it uses one. Or you select a non-live tool, it uses a static one.
This might be a small learning curve for current users, where post processors were hacked to output usable code.
But for new users, there isn't an issue if you ask me.
So if you ask me, the new posts shouldn't actually do drilling with a static tool on the part center when a live tool is selected. That is dangerous in my opinion. You select one thing and another happens.
But you can, of course, add such a message to the posts of your customers.
Laurens Wijnschenk
3DTechDraw
AutoDesk CAM user & Post editor.
René for Legend.
@Laurens-3DTechDraw. There is a big difference between selecting the right tool diameter and forgetting to uncheck "live tool". Live tooling is invisible from the CAM tree, and you have to click 4 times from the CAM tree to see this. During every of these 4 clicks, the diameter of the selected hole and the diameter drilled by the choosen tool is visible, so regarding security totally uncomparable.
I've seen it happen a few times now, even though I explained the live tool checkbox. In case of a Haas ST10. You don't select a live tool: You select a position in the turret, the machine turns on the motor for the live tool, but because in this case there is no connection with the static drill, that is in the mentioned pocket, the drill will crash into the piece.
The dev team in HSM decided to put live tool drilling and static drilling in the same operation, while they are totally different regarding machining. It makes programming easier, but recognizing the difference/potential error harder.
You can fix this in a number of ways:
*Warning in every millturn post like mentioned
*Indicate in a drilling operation on X0, with mill/turn in the setup wheter its a live tool operation
*Indicate in the CAMtree, with a mill/turn setup whether its a turning or a milling operation
Inventor HSM and Fusion 360 CAM trainer and postprocessor builder in the Netherlands and Belgium.
For now there is no way to alert the user in the user interface since there is not information. The live tool setting was added to avoid having the posts guess what was intended. So if you never use live tools for a post you could make the post fail in the case to avoid problems. But other than that it will be tricky to make something will fit everybody. That said, the live tool setting could be made more clear in the future if we make a turret / crib assembly feature. That would allow it to be more visual what the tool capabilities are. If live tool is set for the tool, the expectation is that the post will use the live tool (or fail if unsupported).
I have opened ticket CAM-7934 for presenting the live tool setting / X0 for Drill operations in mill-turn mode.