Skip to Content

SiePortal

The integrated platform for your product selection, buying and support workflow - bringing together Industry Mall and Online Support.

SiePortalDeutsch

Search

Home
Support Support
{{(apiData.Support | filter:{'rank':1}:true)[0].title}} Support
- Menu temporary not available
- Menu temporary not available
- Menue temporary not available
- {{item.title}}

Products & Services
- Menu temporary not available
- Menue temporary not available
- {{item.title}}
Support Support
{{(apiData.Support | filter:{'rank':1}:true)[0].title}} Support
- Menu temporary not available
- Menue temporary not available
- {{item.title}}
MySiePortal MySiePortal
{{(apiData.MySiePortal | filter:{'rank':1}:true)[0].title}} MySiePortal
- Menu temporary not available
- Menue temporary not available
- {{item.title}}
Cart ({{apiData.CartCount}})

Navigation

Error in end point of circle while grinding cam

Created by: Ruselgun at: 2/27/2009 8:44 PM (6 Replies)

Rating (0)

Thanks 0

7 Entries

2/27/2009 8:44 PM	Rate (0)
Ruselgun Posts: 6 Rating: (0)	Hello, Please see image showing the axes in the attachment first (ekseni means axis). I want to grind a cam, what i am doing is; In autocad i rotate the cam shape at 1 degree intervals, and get the position of the grinding wheel (which moves only on the x axis) at tangent points then draw the c-v axis profile (you can find in the attachment), later from this profile i get delta c and delta v values (i work incremental) and get arc radius values and write the code below, but i gives Channel 1 block N004 error in end point of circle error. From the error description i found MD 21000=0.01 and MD 21010=0.001, i don't know where i am making mistake. The values are very precise as you can also check by dist command in autocad. CR is in degrees, as you can find from the properties of the most left arc. I will be very glad if you can help. Thanks, G01 G91 G64 N001 X=-0.05 F=R380 N003 C104 V=0 F=R380 G1 C0.0 V0.0 N004 G3 C=8.96465499 V=0.12910664 CR=336.35941839 F=R380 N005 G3 C=11.203455 V=0.28722069 CR=516.41059566 F=R380 N006 G3 C=3.34981839 V=0.27460651 CR=33.8451579 F=R380 N007 G3 C=3.30925883 V=0.59079732 CR=40.41994819 F=R380 N008 G2 C=13.04532732 V=3.26488826 CR=247.19478315 F=R380 N009 G2 C=8.80678814 V=1.68039389 CR=165.96347604 F=R380 . . . . . Attachment test.zip (238 Downloads)
Ruselgun Posts: 6 Rating: (0)
Suggestion To thank Quote Answer

2/28/2009 5:57 PM	Rate (0)
Jason. Experienced Member Joined: 7/13/2008 Last visit: 1/16/2025 Posts: 107 Rating: (9)	Are you the builder or end user? Some part programmers prefer to use a curve table definition to establish the cam relationship, but that is an option, and I don't think it is allowed on the export version of the software. Depending on the destination of the machine. Have you had any success making a circle betwen the C axis and V? I can only guess that you are using G19, and the machine is configured like a lathe at that moment. I expect (V or X) and Z is in the geometry grouping, so you could circular interpolate between VorX and Z. Not with C. If the C axis is not in the geometry grouping circular interpolation would not be carried out with C as a default. You need to read about the transmit function, and see if your builder has set this up on this machine? Additionally,if you don't have cases where you need to grind past zero, you may want to verify if a machine data to make only solutions one one size of V o rX 0. It would be bad to grind through the part.(MD24911 $MC_TRANSMIT_POLE_SIDE_FIX_1 this may need set up depending on how the machine operates) Once you have a transmit transformation created, you can activate the transmit function, and cirularly interpolate between the C and (V or X), but it will look like the examples in doconcd.
	Last edited by: jason.polensky at: 2/28/2009 6:00 PM
Suggestion To thank Quote Answer

2/28/2009 9:04 PM	Rate (0)
Pee Ell Sea Posts: 672 Rating: (57)	HI, It looks like you are trying to do circular interpolation using a rotary axis and a linear axis ? My guess is that you do not need the g3 command. Just interpolate between the c axis and the V axis.
Pee Ell Sea Posts: 672 Rating: (57)
Suggestion To thank Quote Answer

3/1/2009 8:10 PM	Rate (0)
Ruselgun Posts: 6 Rating: (0)	Hello, I am an end user, we are using G18, Z axis sets which cam will be grinded on the same mill. On one cam c axis is the rotary axis, the cam rotates about this CCW, and the wheel only moves on the V axis. Am i making a mistake to interpolate between a rotary axis and a linee axis? If we could have done this, we would have gotten perfect cam shapes. İf you can write example code i will be very glad, i am very new to this sector, sometimes i don't know exactly what i am doing. Looking forward for your precios helps. Regards,
Ruselgun Posts: 6 Rating: (0)
Suggestion To thank Quote Answer

3/2/2009 1:18 AM	Rate (0)
Jason. Experienced Member Joined: 7/13/2008 Last visit: 1/16/2025 Posts: 107 Rating: (9)	Look in the Programming Manual Job Planning, there is an example there. https://www.automation.siemens.com/doconweb/showpdf.asp?mw=0&lword=transmit&rword=&sop=0&sac=default&spg=0&item=19&cd=sinumerik_simodrive_10_2008_e&scope=all&ResultSet=3929548,3929549,3929550,3929551,3929700,3929701,3929702,3929703,3929704,3929547,3929553,3929554,3929555,3929556,3929557,3929558,3929559,3929560,3929561,3929562,3929563,3929552,3929533,3929534,3929535,3929536,3929537,3929538,3929539,3929540,3929506,3929507,3929508,3929509,3929510,3929511,3929512,3929513,3929514,3929515,3929516,3929517,3929518,3929519,3929520,3929521,3929522,3929523,3929524,3929525,3929526,3929770,3929771,3929764,3929765,3929766,3929767,3929760,3929761,3929762,3929763,3929815,3929816,3929527,3929528,3929529,3929530,3929564,3929565,3929566,3929567,3929568,3929569,3929570,3929571,3929572&CurrentItem=3929513&ResultType=search You are close in your program, if your machine supports transmit. Except you will be using xy coordinates, instead of xc.

Suggestion To thank Quote Answer

3/13/2009 12:16 PM	Rate (0)
Ruselgun Posts: 6 Rating: (0)	Thanks so much, in case of using xy planes, will both x and y planes refer to lineer axes, or y will be rotary axis? As you know we have rotational angle values vs vertical wheel movement values, in grinding operation. Regards,
Ruselgun Posts: 6 Rating: (0)
Suggestion To thank Quote Answer

3/16/2009 5:36 AM	Rate (0)
Jason. Experienced Member Joined: 7/13/2008 Last visit: 1/16/2025 Posts: 107 Rating: (9)	The y is imaginary. It is created by moving the spindle around with the X. If your builder expects that you can make a cam with that machine, they may have an example more directly what you are looking for.

Suggestion To thank Quote Answer

|

Share this page:

Share this page on...

Follow us on