Multicam Feed Rates

[benjamineEK8P2]

We recently purchased a 3-axis multicam cnc router. We can use enroute to run the machine fine.

My company has much more experience with fusion and rather use that for cam. The problem seems to be in our tests with cam produced in gcode. The machine is ignoring the feedrates that we have set up in cam.

We have the spindle speed at 18000 rpm

The feed rate will be set at 36in/min

Run the file and the machine will run it at 1000in/min which is it's max for the machine. It will slow for corners but ramps right up to 1000in/min when it can.

Has anyone else encountered this or know of a solution. I'm leaning on the side of user error because we're still learning or even bad posts for the machine.

I've search the forums and turn up no answers.

Thanks

[LibertyMachine]

I'm also leaning towards user error. Do you mind sharing your .f3d file as well as the post you are running?

To export an .f3d: File > Export > Define location to where to save it to > Click OK. Reply to this thread and attach the file

[HughesTooling]

This could be something simple like the feed having the wrong feed format. I have a machine where the feed has to be a whole number without a decimal point, if it has a point it's ignored and all moves are done at the machine defaults or the last feed that was set correctly.

Mark

[LibertyMachine]

@HughesTooling is this a modern or dated piece of equipment? I'm suprised that a modern machine (with a modern control) would have such a requirement. Years ago, I had the (mis)fortune of running a very old turret lathe with a bubble memory control. That was the same way, no decimal permitted. Fun times indeed....

[HughesTooling]

---

@Anonymous wrote:

@HughesTooling is this a modern or dated piece of equipment? I'm suprised that a modern machine (with a modern control) would have such a requirement. Years ago, I had the (mis)fortune of running a very old turret lathe with a bubble memory control. That was the same way, no decimal permitted. Fun times indeed....

---

Thinking about it a bit more, it was an old AHHA control on a lathe, I replaced it last year. I used a couple of differnt CAM systems with it over the years and this would always catch me out.

Mark

[benjamineEK8P2]

I'm attaching one of the files that we have run along with the posts. Using the generic multicam.cps

[benjamineEK8P2]

Our feedrates that were inputted don't have decimal points. Don't believe that's the problem but overall I think your assement is correct. It looks like its running its machine defaults.

[LibertyMachine]

Do you have a program that has been run before, produced by another CAM package or perhaps shipped with the machine?

[Anonymous · Accepted solution]

HI @benjamineEK8P2

We also have Multicams and it's important to note - they run in IN/SEC not IN/MIN! Enroute translates the in/min to in/sec when it outputs the G-Code but Fusion doesn't.

The defualt fusion post sends them out in IN/MIN which the machine interperates as IN/SEC making it max out on feed!

Test this like this: Take your feedrate (say 60 in/min) and input it in Fusion as in/sec (in this case, 1 in/min) then run a few more tests. You'll see it works much better.

Hope this helps!

[benjamineEK8P2]

This is a post created in enroute that ran with the correctly assigned feedrates

[Anonymous]

Yep, you have the same issue I did...Look at your EnRoute file at the lines with "F"

You have F0.38, F1.2, etc.  this is Feedrate - 0.38 in/sec, Feedrate 1.2 in/sec.

Your Fusion file has F80 F90 - 80 in/sec, 90 in/sec, faster than the machine goes.

What you need is either

- Your Post changed so it translates in/min to in/sec (divide by 60)

- Set up your feeds and speeds for in/sec (don't need to change your post for this).

I just did the second one. In Fusion, it states in/min, but I know I need to input in/sec, so that's what I do.

Good luck!

[benjamineEK8P2]

This was completely the case of fusion being in in/min and multicam routers being in/sec. Now I feel a bit silly for noticing the units difference. I divided all the feedrates by 60 and ran it. The machine ran at a correct feedrates.

This made my day and thanks for everyone's help.

[Funkier9000]

If I wanted to customize the multicam.cps post to divide all feeds by 60, how would I do that?  I've looked at the source code but wouldn't know where to insert a "/60" into the feed portion.  

Or, is this something Autodesk should correct globally for everyone's multicam.cps?

[Anonymous]

I operate a 3-axis Multicam 3000 cnc and also experienced feedrate issues with the canned Fusion post processors, ie. the feedrate speeds run away and plows the bit through the material at 1,000-1,500in/min.  as an experiment i slowed the feedrate on my tooling to a crawl @1in/min and the machine still runs terrifyingly fast (+1,000in/min) when cutting into the material so i don't think it's a matter of simply converting the feedrate from in/min to in/sec (or mm/min to mm/sec).  however, what is even stranger is the cnc seems to respect the proper ramp speeds but once it hits the cutting depth it resumes light speed.  

i haved generated .cnc files using Vectric Aspire and VCarve Pro for the past 5 years and have never experienced any  issues controlling the feedrate speeds.  all of my Vectric files (.cnc) are set to in/min for feedrates and that is what our machine seems to prefer.  i am not a G-Code wizard so i would like to know how to remedy this feedrate problem b/c i want to take advantage of the more advanced 3D toolpathing in Fusion but we can not get the .ISO or .HPGL posts to cooperate with our cnc.  when i load the Fusion generated .HPGL post files my artwork actually scales down to about .0001mm for some reason so i never even bothered trying to run those files.  the .ISO post preserves the scale but as mentioned before the feedrates are out of control... 

[rob.r.martineau]

Hello

We just got our multicam 3R, and it looks that i have de same bug with the feedrate in the post. For an ask of 200 inch/min, the machine cut with a feedrate around 1200 inch/min. Have you find a solution yet?

[chargiss]

Has anyone been able to come up with an answer to this question?? I'm having the same issue when posting programs from HSM to my multicam 3000 series router. I've looked over the code very closely and everything looks good, but when I try to run it the feed-rate is ridiculously high. I even called multicam tech support and they didn't know how to fix it. Please help!!

[rob.r.martineau]

Hi chargiss
In the post-process window, choose ''Format'', than change the feedrate time unit for ''second''. Multicam calculate in second.
It works for me.
good luck