Multicam Digital Express

**FSdigitalla** · 09-25-2016, 12:56 AM

Hi Guys,

I have a small shop and we only cutting graphic.
Any one have a problem with machine jerkin, shuddering when it making small circle / eclipse or even a curve?
Been addressing this problem to tech but they keep saying it's on the file.
I'm using enroute for this digi express and we clean up countour 0.03 everytime we encounter circle or small eclipse.
File i'm getting is dxf file.

Any1 have encounter this kinda problem and have resolution to it ?
Sometime when we want to cut a perfect circle it just never happen.

Thanks in advance for any input or opinion

Similar Threads:

CNC Express SQ
Need Help!- v21 express
Need Help!- NX CAM express

**MCPservice** · 09-26-2016, 07:15 PM

Have you ran a older program that you know works to see if this shows up also?

**FSdigitalla** · 09-27-2016, 03:14 PM

Hi MP,

No we always ran this multicam with enroute.
I just notice it maybe the machine can't handle the segment regarding accel and deaccellerate every segment so machine make a sudden stop and moving at the same time.
It will make that jerking problem. Never a smooth curves.

**keesfrees** · 09-27-2016, 06:01 PM

nice to see some activity here

it's my guess you're dxf contains lotssss of small line segments to make a curve, instead of curves made out of arcs
the multicam controller doesn't like this at all

can you have a look at you're g-code, maybe post a sample here
when you open you're gocde in jobpreviewer you can have a look at the info to tell whether there are (many) arcs involved

**Routerfiend** · 09-28-2016, 12:39 PM

Hi
Yes have the same problem!! I have three Multicams 1 MG & 2 5000 s and the newest one ( About a year old ) does it too. I have the CNCworld tech guys looking at the problem and speaking to Multicam U.S. The best they`ve come up with so far is to increase the chord tolerance , which I`ve done. It`s better but still not great. I use Alphacam to create my programmes and the guys there don`t quite have a grasp on the problem so it`s still ongoing. Also muticams don`t like helical interpolations either , a disc cut in alliuminium will have the look of a worn sprocket. I do a lot of tool making and surface machining is a bit of a problem. Even running in fresh air the whole thing judders regardless of feed rate. It`s better in some directions than others and dependant on the size of arc being cut. I made a demo programme using polyline & spline arcs of various sizes in XYZ and the transit through the arc is terrible. Muticam say that the problem is in the way Alphacam outputs the code . An arc being made up of a lot of small straight lines and that it`s the acceleration and deceleration through these points that Multicam doesn`t deal with very well. If they come up with a solution I`ll post the results.

The best I can offer at the moment as a partial cure is to slow your federate down to a crawl for small holes and if your cad package allows use a helical down feed. It`s not perfect but it will stop your machine from shaking itself to bits !!

**keesfrees** · 09-29-2016, 07:11 AM

the multicam control doesn't support a gcode for "Path Control Mode" (or has it been added later, can't find it on the web)
on other controls G64 is used to set a compromise for speed <-> accuracy

so you need to tweak the parameters in you're control using MotionMechanic
before you do anything make a copy

from machine -> file : shift + F2
( from file -> machine : F3 )

these are the params of interest :

Arc Speed Factor 193 F 4
Arc Work Radius 194 F 25
Arc Minimum Velocity 195 F 12
F means float
the value after F is my current value which is good for me in most cases

on the command line of MotionMechanic :
193 get_float f.
will show current value
5 193 set_float
will set param 193 to 5

there used to be a lot of info on multicam.com
and a forum, not any more though . . .

**keesfrees** · 10-12-2016, 05:58 AM

dear FSdigitalla,

I don't mind spending some time on typing, would be nice to know though wether you've made any progress on this

thanks !

**Boltz** · 11-09-2016, 05:07 PM

Originally Posted by keesfrees

dear FSdigitalla,

I don't mind spending some time on typing, would be nice to know though wether you've made any progress on this

thanks !

I've tried for years to find out what the parameters do. Where did you find that?

**Rainerio** · 11-29-2019, 11:33 AM

Hello, I have a multicam, stopped working, reinstalled suite 4 and after loading the machine .xmi file, shows the following message on controller (1). Would you help me? Is the procedure just loading the .xmi file or should I do another procedure?

(1) Please Wait ...
Loading
Version 8. 19

But it never finishes loading.
Please.