What's new
What's new

FUSION 360 Machine Simulation (Lathe)

MaYahia91

Plastic
Joined
Jan 11, 2024
Hello Brothers,
I just started a new role with a new company used Autodesk Fusion 360 as a CAM software.
I'm a CNC Programmer specifically in Turning and Mill-Turn
but when I'm using Fusion 360 there is some points I want to understand
1- Why there is not any template machine for lathe?
2-There is no simulation when I programmed Sub-Spindle
I need to Build a Machine to Make machine simulation and check if there is something wrong or any collision or not. because the technical office is in the country where I am working in, and the machine is in another country.
so, I can't see the machine running.
How can I start building machine? any advice?
 
1- Why there is not any template machine for lathe?

Correct observation because there is no lathe simulation in F360 to this date.

It has been teased with the machine builder V2:

I do not know the actual timeline or when this will be released; the lathe simulation is still unavailable even to the resellers in the "alpha testing stage".

If you want to program millturns, there are better choices than F360.
I presume it will take years of user feedback before this thing is even somewhat usable on basic ZX lathes.
It's unclear at this point if it can ever support advanced kinematics to perform simulations for more complex mill turns in the distant future. (Be it multi-channel or, LSY or B-axis machines.)

Given that, you should look elsewhere for a different CAM.

I will also bite my tongue regarding using only CL data and running a machine in another country; good luck to you.
 
thank you, guys, for your support.
You are right @MAWO I Should looking for another Sofware for turning and mill-turn.
what do you think about the better Sofware for these jobs?
Esprit Cam, Siemens NX or another Software?
 
thank you, guys, for your support.
You are right @MAWO I Should looking for another Sofware for turning and mill-turn.
what do you think about the better Sofware for these jobs?
Esprit Cam, Siemens NX or another Software?
NX, MCAM, Esprit, Top Solid are all contenders. NX has its own G code simulation built in.

What about external simulators like
Vericut or Roboris Eureka G-Code or Pimpel CHECKITB4.

Maybe check them out.
 
Auto desk bought camplete. That should handle your lathe simulation from what I understand. Never tried it myself.
F360 seems very mill focused.
I just started using it for a sub and y axis lathe this week.
Will have more to say in a year I guess
 
Let's not get ahead of ourselves here; we are painting this topic with a broad brush.
I hesitated to reply because I didn't want to come across as a jerk, but here it comes.

You are right @MAWO I Should looking for another Sofware for turning and mill-turn.
what do you think about the better Sofware for these jobs?
Esprit Cam, Siemens NX or another Software?

First, OP, where are you from? According to your profile, Cairo, like in Egypt? Like in Africa?

We could go on pages about the best solution to program mill-turns in our individual case, but our advice could as well be useless to you, given your location.
So while NX, Esprit, Gibbs, Topsolid, MasterCAM, Solidcam, or whatever might work for someone in his geographical location, it could as well not work for you.
I do not know how well these are represented in Africa, but OP's ''mileage'' will vary mainly according to that.

Secondly, this is an almost irrelevant question because we would need more data from you. It's the same as asking what's the best car? Well, it depends, really...

I could write you about how we made millions running Integrex and Esprit, but this information would be only helpful to you if you have support for both Esprit and an actual Integrex...
So first, we need to find out what lathes and mill-turns you would be running.
We don't know if you are programming for a single spindle c-axis lathe with live tooling, an LSY, a twin-spindle twin turret, an ATC B-axis machine, or some super 11-axis INDEX TRAUB with dual lower turrets and ATC B-axis head.

What machine is it / are they? Make? Model? Control?

Second, we do not know what features you will be programming.
There is a big difference between programming a couple of radial holes and a few flats for a wrench / doing full five-axis work or gear skiving... The work you will be doing will sometimes define the choice of CAM alone.

Second, you should research who is represented in your area and has good references. My advice for the CAM package you should choose, even if you do not know what you will program for, is to select the one you can get local support and training for and choose a provider that can provide you with a post.

Regarding machine simulation, pardon me if I am wrong, but you seem new to this.
If you have a good post, Fusion is still ok to program basic things for an LSY lathe. But you must pay for this post and have it proven on the spot on the machine.
The question still is if there are any local AD resellers who could help you with this. But at this time, as I have mentioned, you will not have the kinematic simulation.

The second stage is kinematic machine simulation in CAM, which is more or less present in all the packages mentioned above.
Again, somebody will have to set this up for your machine with your post.
This simulation does however generally rely on CL data, so it does not in some cases account for things like probing cycles or canned cycles, and its level will depend on the CAM package you are running.
At this stage, we are also getting to the point of how well-detailed you want to have the simulation.
If you want just basic sheet metal and kinematics or to model the jaws and chucks, use solid tooling models, etc.
Create a digital twin of your real-life setup as closely as possible.

The third stage is full-on G-code-based simulation, with everything modelled and the machine running on a virtual controller.
While this is beginning to be popular on the 5-axis, on Mill-turns, it can still be a mixed bag, depending on what you choose and what machine you are running.

No offense, but you need to consider why programming for somebody on a machine in a different country is a bad idea. Whose fault will it be when the machine crashes? Yours, or the setup guys?
Because even if you would have the latest and greatest perfect full-on G-code simulated digital twin, the guy setting the machine up still needs to set it up the same way you have it in your CAM / Digital twin.
This means respecting the tool stick-out, positioning the tooling blocks on the turret, using the same jaws, etc. Assuming you are asking how to simulate a lathe in Fusion here, it could be too much to bite off at once. Also, for example, if the raw blanks are oversized, you will never catch them in your digital machine if they are in another country.

My setup guys, still open Esprit next to the machine to set up some of the more complex jobs; you cannot even set them up according to the setup sheet anymore.
This means to make sure it does not crash, the guy setting up the mill-turn would have to have a copy of your simulation.

And yet, all it will take to crash the machine is one wrong offset... It would be best if you reconsidered this idea; it might be too much to get into at once.

TLDR: We do not know who is local to you or who has good references.
Get somebody who can teach you the chosen CAM system in person, train you, and guide you through this process, and will make you a post for the machines you will be using.
In this case, the best CAM system for mill-turn is the one you can use and have support for.

There are already too many threads here on how to get started in Esprit / NX
. It's a professional piece of software that costs a lot of money.
DO NOT RELY ON YouTube or forums; get in-person training for your use case.

What about external simulators like
Vericut or Roboris Eureka G-Code or Pimpel CHECKITB4.

Maybe check them out.
While the folks at Pimpel are superb, they are superb if you are local to them or, let's say, at least somewhat local to them...
That is the main reason to choose them: they will spend time with you on the shop floor making sure everything is correct. That is not exactly OP's case.

Second, CHECKITB4 is currently a viable option only for Siemens / HH; Fanuc is presently in development and unavailable.
Third, I was hesitant to recommend a kit of software that is 50k+ or easily more, depending on the application, if he is currently using Fusion and has a few other issues before he can get going.

Auto desk bought camplete. That should handle your lathe simulation from what I understand. Never tried it myself.
F360 seems very mill focused.
I just started using it for a sub and y axis lathe this week.
Will have more to say in a year I guess

Yeah.No, not really.

Camplete TurnMill, is only viable for NT machines.
Unless the OP is running a Nakamura, it would be utterly useless to him. Turnmill was supposed to be the prime simulation/post-processing solution for Nakamura Tome multitasking machines.

Second, since Autodesk bought Camplete, they made TurnMill an orphan.
The only reseller providing this service anymore in the US is Multiaxis, and AD being Autodi... You cannot even buy it in Europe; Multiaxis is limited to supporting only US clients due to AD being di... (Ok, you can buy it in Europe, but AD will refuse any support or training at all.)
In England, you can get support from Multiaxis through ETG, which is a Nakamura dealer.

Hence, it is useless everywhere in the world, apart from the US and UK, because you cannot legally use it. (There is a workaround: if you would happen to have a registered US company, Multiaxis could support you, but I don't really want to get into working around license agreements...)

So if you are in the US or UK, you can go with Camplete TurnMill, if you are anywhere else in the world, and have a Nakamura, your mileage may vary.
Also, for practical reasons, it might not be best to have only online support across the pond for your 3-turret lathe :)
The only reason this still exists is that Methods, used to bundle these as an out-of-the-box solution for simulating and post-processing your Nakamura, and they sold quite a few, in the US and got people used to it.

Third, the workflow could be more optimal in this day and age.
You export CL data from Fusion and then do your synchronization, wait for codes, rotary control, and post-processing of the final program in Camplete.
This means you have to do things in two software packages, and if you want to change a toolpath, for example, going back and forth, which is not the most optimal workflow.
I largely prefer to do the twin turret stuff like pinch / follow, turning in CAM directly, and not synchronizing those in a separate program for the already stated above reasons.
 








 
Back
Top